Q1. How do I generate automatic solder paste Gerber files?

EDWinXP do not have solder paste layer assigned by default, SMD packages have only solder mask and component layer items in the pad stacks.
Select one of the layers (ex: A) as solder paste layer. Then add necessary item (rectangle) on this layer to pad stack for these pads in the packages.
Select one of the top layers (A-M) remembering that if components are flipped to the other side of the board then items from top layer are also flipped symmetrically to the bottom. Those on component layer are flipped to solder layer, from A to Z, from B to Y etc etc. “Symmetry  line” for this flipping is located between layers M and N meaning that items from M layer flip to N.
So it must be remembered that paste layer for components mounted on the bottom side of the board would need a separate layer for bottom solder paste. This will be handled automatically. If (ex: A) layer is selected for top solder paste layer then (when component is flipped) solder paste layer item(s) in the pad stack will wind up on Z layer.  It also means (in this case) that Z layer is reserved for bottom solder paste and should not be used for placing traces.
To plot solder paste layer(s) properly on the Gerber, one should suppress plotting of PMD pads in the fabrication set ups for these layers.

Q2. The PCB Company I use to have my boards fabricated now offers a solder silkscreen option. Is there any way to generate a solder paste file using EDWinXP 1.20?

With solder paste files means Gerber artworks presenting spots where soldering paste has to be applied before spot soldering SMD pads to the board.
You have to select one of the layers (ex A) as solder paste layer. Then add necessary item (rectangle) on this layer to pad stack for these pads in the packages.
You have to select one of top layers (A-M) remembering that if you flips a component to the other side of the board then items from top layer are also flipped symmetrically to the bottom. Those on component layer are flipped to solder layer, from A to Z, from B to Y etc. “Symmetry line” for this flipping is located between layers M and N meaning that items from M layer flip to N.
So it must be remembered that paste layer for components mounted on the bottom side of the board would need a separate layer for bottom solder paste. This will be handled automatically. If someone select ex A layer for top solder paste layer then (when component is flipped) solder paste layer item(s) in the pad stack will wind up on Z layer. It also means (in this case) that Z layer is reserved for bottom solder paste and should not be used for placing traces.
To plot solder paste layer(s) properly on the Gerber, one should suppress plotting of PMD pads in the fabrication set ups for these layers.
Since we do not have solder paste layer assigned by default, SMD packages have only solder mask and component layer items in the pad stacks.
There are two different technologies for mounting SMD components. One is spot soldering where you need solder paste layer. The other is gluing with conductive glue. In this case you need a layer to store items that represent clicks of adhesive. This is equivalent to solder paste.

Q3. The Edwin drillfiles (like the one attached) declare the drill sizes at the start of the file, like this:
...
;PATCH- 0   
;TOOLS USED (INCH / MM) 
;T01-0.014 / 0.4 ( 238)  
;T02-0.020 / 0.5 ( 262) 
  ;T03-0.024 / 0.6 ( 160) 
  ;T04-0.030 / 0.8 ( 4)  
;T05-0.032 / 0.8 ( 2)  
;T06-0.035 / 0.9 ( 17)  
;T07-0.040 / 1.0 ( 24)  
;T08-0.100 / 2.5 ( 2)  
;STOP
;T01-0.120 / 3.0 ( 5)  
;T02-0.130 / 3.3 ( 2)
   ;STOP
FMAT,2
INCH,LZ
T01C0.014
T02C0.020
T03C0.024
T04C0.030
T05C0.032
T06C0.035
T07C0.040
T08C0.100
T09C0.120
T10C0.130
... In the file, the reference T01 is used twice, for the 0.014 hole and for the 0.120 hole.
In the past, I have had troubles with the PCB fabrication, because they omitted the STOP command and therefore used the 0.014 drill also for the 0.120 holes. Since then I added a text file with warnings.
  However, now the next problem shows: I have a Gerber Editor to verify the output files and make small (copper) changes when needed to improve the PCB even further. But this program can not deal with the STOP (of course).  
Question:
1) Is it necessary to use these STOP commands in Edwin?
2) Is it possible to change (a setting) so Edwin directly generates the proper drill file, without the STOP commands?


Edwin puts stop after every 8 different tools because tool magazine capacity (for drilling machine) is set to 8. User may set this value to some bigger number and in this way there won't be any stops within.
Fabrication Manger → Fabrication → Setup → NC drill Data → Tools → Tool Magazine Size.


Q4. Trying to load/import a symbol into the schematic editor:
  Process taken:
  Tools:       Component
                Add component to the ckt (CC)
                Explorer to add component (F1)
                Select Symbols
                Misc. Symbols
                Relay
                Ctrl - L/Click  to Drag
                Result
                  An O with a \  shows up on the editor but no symbol.

Components can be loaded to Schematic Editor only from Part .It cannot be done from Symbol. To load Relay to Schematic Editor executes the following steps:  Go to FETRELS.PART in Library Explorer, the following window appears.


Select the required RELAY and load to Schematic. In MISC.part component can only be loaded to Layout Editor.

Q5. I use Edwin XP Pro 1.30 and it is not clear how I can control if a hole is plated or not plated. How can I control that?

It is controlled in two ways.
For every hole you can assign so called “hole category” in range from 0 to 7.  Holes of the same category are grouped in single path inside drill output file.


By default all holes in pads have “ hole category” set to 0. By convention it is assumed that this category groups all holes that are plated.  You may select any other category for non-plated holes. 
Drilling of plated and non-plated holes is done in two separate operations. First, the plated holes are drilled. Non-plated holes are drilled after plating operation is completed.
So you need separate NC-drilling programs for each type of holes. If you for example assign hole category = 1 for non-plated holes and 0 for plated holes, the program will generated NC-drill output containing (within one file) two drilling programs ( we call it patches in FM) – first for category 0 and after that for category 1.



Q6.The problem is that sometimes holes are missed when designing rings. Please find attached the a file underlining rings (blu) without hole (pink).
The via #2 present in the project is having very small hole dimension to get drilled with the drill machine set. The error in the project might be because of the holes for that particular vias are not drilled up. Please check by increasing the size of the vias for drilling.

Here 35 vias are of type #2, also few other drill points were skipped of from drilling.

The padstack/ vias size of the #2 via was set as below

Q7. The problem occurs also with Vias #1 (larger), and with Vias #2 not always.
The remedy is that, the user should use suitable vias (here in this case the vias is 2) of identical dimension respectively which is compatible for the tools in the patches/hole category for drilling. Please also check whether any pad holes of the components placed in the layout is having a very low hole diameter such that it not drilled. All other drill points seems worthy.

Q8. If the vias are not suitable, why many times it works? Only sometimes the hole is missed. However it does happen also when the diameter is bigger (#1). For your info the number of holes registered in Fabrication Manager / Statistic Information is different to the number of holes in NCDrill. What the customer asks is that could be helpful at least to have an indication of where a hole is missed.

Please unbury the vias in the fabrication manager. This can be performed from Fabrication Manager → Tools → Unbury Vias and then create the NC drill.

Q9. I cannot fine any default circuits which would prevent creating the List.

The problem occurred because the components in your project were not packed. The List of materials can only be created after it is packaged.  Please pack all components in the project so that the “Create list of materials” is enabled. After that, please follow the steps from the following mails to create the list. For the components which doesn’t have package, please enter the values manually. Here we are attaching List of Materials file.

Q10.I have been struggling with this problem for two days.  I have combed through the schematic and the project library looking for missing or improper packages, repacked using the (Tools > Block Edit > Unpack / Repack with option F2 selected) procedure, removed all the SPL0 and SPL1 symbols, and still cannot get either the LOM button to come on, or the component packages to to appear on the Layout editor screen.  
I have acquired version 1.40 in the hopes of eliminating a possible "aging" problem with 1.20, without success.  I have also noticed that at least one of the demo projects that came with the system seem to also have this problem.  One project was very small, but when I loaded it, the "Create list of Materials" button would not come on.  Remembering what you said about parts without packages, I removed the VCC and GND symbols from the schematic, and found the LOM button miraculously came on, and the component packages showed up on the layout screen.  This may have been a fluke.    
I have attached the TomsWay file which is a later version of the one I sent you previously.  Please take a few minutes to look at it and tell me what I must do to fix it. Or if you can fix it, return the file to me and I'll try to run it on my system.  That would be very helpful in that I could determine that the problem may be in my old HP XP system and help me regain my sanity.  I'm praying for a miracle.

The “Create list of materials” will be enabled only after the components in the schematic are packed. Packaging can be done automatically from Schematic editor -> tools -> components-> Pack/ unpack component -> Auto packaging (F3). Eventhough the SPL0 and SPL1 symbols are not removed the list of materials will be created. Please pack all components in the project so that the “Create list of materials” gets enabled. Here we are attaching List of Materials file. You can export it into excel format.

Q11. On opening the Help file which you sent, and selecting "Circuits and subcircuits" it shows me a nice clear diagram, with circuit "HA_INT" as a subcircuit of circuit "HA".
This is exactly what I want to achieve (I have used hierarchies extensively in Viewlogic, for Xilinx FPGA design).  My problem is that it does not tell me how to achieve it.
How do I create "HA_INT", or define it to be a subcircuit of "HA"?
I can get the "create/add circuit" option when Project is highlighted in navigator.  But if I highlight an existing Circuit, it does NOT give me the option to create/add circuit (or subcircuit) within it.
I cannot find anywhere guidance on how to define something as a sub-circuit, or, having done so, how to link that subcircuit to a "block" element of a main circuit.
All of the help I have found states what hierarchies and subcircuits are, but NOT how to create subcircuits and link them into a main circuit block/element.
Surely other people have asked about this?  Or do they simply not use the facility?

 For defining hierarchy, the steps shown below has to be followed
1.  Create a main symbol (ex: a block with 2 input nodes and 1 output node) in the Schematic page of circuit MAINHEIR. This will be the top level circuit.
A block can be created from the Library editor and load it to the schematic or the block can be created from Schematic Editor → Components → Add Components to the circuit → Add Block diagram elements (F6).

2. Create another circuit in the same project as Project → Add Circuit. This will establish a new circuit. Let us consider this as the internal circuit.

3. Rename this new circuit as INTERNAL_CKT.
Dr
aw the internal circuit (the internal schematic) of the block diagram in the schematic page of the newly created circuit (INTERNAL_CKT) within the same project. 4. The sub circuit I/O nodes for the nets in the internal circuit can be set next.
Imp: The name of the nets in the main circuit and in the internal circuit should be the same

For this, load the internal circuit schematic and set the sub circuit I/O nodes for the nets for which u want to set the sub circuit tags.
This can be accomplished from Tool → Components → Hierarchy down → Set sub circuit I/O Nodes . Give a suitable name as “Sub circuit name” with description. Then select the nets one at a time from the drop down menu. The description for each of the nets can be given in the text box “Node Description”. Click “Add” to add each of these nets. Finally click “Accept”.


Save this project as circuit file. This can be done from by taking the newly created circuit and right click to enable the option “Save Circuit. “.


5. Now click on any of the node in sub circuit schematic and enable Tools→ Components → Hierarchy Down → Hierarchy up (F1). The hookups will appear automatically.
Once the hookups appear, a link will be established between the Main circuit and the internal circuit. To check this, do the following:
Take schematic page of circuit (MAINHEIR). Select Reassign Hierarchy from Tools → Components → Hierarchy Down and click on the block symbol. The internal circuit will be obtained as the result of this operation indicating that a hierarchy has been established.

Q12. The program crashes every time I try to auto-route wires in the schematic editor. It opens a small window which says "Removing existing connections.." and then it crashes with this message: "Application Failure  edwinxp.exe 2.0.0.311 in edwkrn2k.dll 1.0.0.1 at offset 00001ee9"

Please run the “Liveupdate” from Start → EDWinXP ver 1.40 → EDWinXP → Liveupdate so that the files get updated. After this procedure, please check whether the error is recurring.

Q13. I was trying to use the fabrication manager to import the gerber files but seem to fail once it looks for the aperture values.  Would it be possible for you to have a look at the example provided and detail the process of how this would be done in EDWinXP

Please paste the attached file in Drive:\EDWinXP\SYS and generate the artwork files from the gerber. Here these files are in old gerber form (RS-274-D) and that means that aperture list is not embedded.


Please select the “Aperture table” as VIPLCUSTOM.APT and do the artwork generation.

Q14. The client that I’m talking to has a number of these older gerber files along with EEDIII files and want to make sure that they’ll be fully supported for with EDWinXP.  Is the process of creating a custom aperture list something a customer would be capable of, or would he need to have all the current files sent and have it supported via Tech Support?   Also, once the file is visible in fabrication manager, is there an easy process of reverse engineering the board and capturing the schematic?

The user can create their own aperture list from System -> Aperture Table Editor -> Load the existing aperture list and edit it according to the necessity and save with a new name for generation of apertures.

Q15. I am trying to use parts which I created for another project.  How do I access them for a new project.  I have v.120, SN 1209201.

The custom part can be saved to another new library for loading to a new project.
For eg: If AAA.Part is the part library, it should be saved as Library Explorer → File → New → Part Library → Give a name to new library. Then copy the contents from the custom part library by Right click ,Select all , Copy and then Paste it to the new library. By the same way, copy the custom 'Symbol', 'Package' and 'Padstack' libraries to corresponding new libraries.
Please add them to the "Search Sequence" for loading the Parts.
This can be accomplished from EDWinXP Main → Library → Library → Explorer → View → Search sequence → Right Click → Select All.
Follow this procedure for 'Symbol', 'Package' and 'Padstack' tabs so that the corresponding symbols, packages and padstacks are also added. Click on "Accept" to get the changes in effect.
After these procedures, the components can be loaded to new project.

Q16. I attempt to resume my work on the OVH737-0.epb project that you have fixed some days ago, but i can't do almost nothing. I need to add some LED in the MAINHIER board, but when i try to connect in layout i still have problems. EDwin find failing connections, delete traces that have not relation with the connection where i work in layout, delete complete connector in schematic... I worked with ED for many years on my previous employment (EED3, EDwin, EDwin32 EDwin2000 and xp) and never had these problems, what happening??? System is updated.

Please run the Liveupdate utility inorder to get updated with the latest files and check whether the error persists.The Liveupdate can be invoked from Start → Programs → EDWinXP ver 1.40 → EDWinXP Liveupdate. Or please download the files from the link http://www.edwinxp.com/Files/NetIntegrityFix.zip and unzip and paste to Drive:\EDWinXP (installation folder). Please backup the existing files before it is overwritten.

Q17. I wanted to change a symbol after I had loaded it onto the schematic.  I removed it from the schematic and compacted the Projects Parts file.  The Part file, upon examination, indicated that the part had been removed.  I subsequently checked the Project symbols file and found the symbol still in the Project file.  I was not able to delete it. (I was under the impression that compacting the parts file also removed the symbol associated with the part.) I then accessed the part from the custom part file and opened the part to edit it.  I removed the previous Group 1 symbol. and assigned the new symbol to the part, made the pin assignments,  and saved the part, with a new part name, to the custom part file. Later, I opened my project file and opened the schematic for editing.  I opened the Custom.Part file from the schematic, and loaded the part that I had just assigned the new symbol.  When I moved the part file to my schematic, the old symbol appeared on the schematic!!! I went back to examine the Custom.Part file and reopened the part for editing, and found the Old symbol again associated with the part.. I have read and re-read the manual, and I still have no clue as to what's going on....or how to fix the problem.  I probably have an outdated manual since he screen shots in the manualare not found on the screen.   I would be very appreciative if you could take me through the steps to change a symbol of a part so that the altered symbol appears when I attempt to load the updated part onto the schematic, and not the old symbol.

Please assign the Part with the new symbol and place the new symbol library on the top of the search sequence from Library Explorer → View → Search Sequence ,Move your new symbol library up using the Up arrow, or make the old symbol used in the part Unchecked. Q18. I have a problem when trying to delete a node in the layout program. The system crashes every time I pick this command then pick the pad. This has happened many times on different parts and different files. The problem is definitely localized to this command. Do you have a solution or a software patch?

If you are working with EDWinXP version 1.40, please run the Liveupdate utility inorder to get updated with the latest files and check whether the error persists. The Liveupdate can be invoked from Start → Programs → EDWinXP ver 1.40 → EDWinXP Liveupdate.

Q19. I am intending to upgrade the PC I run Edwin on. How do I go about moving the licence from the old machine to the new ?

Please take the backup from the EDWinXP folders → eg: LIB, JOB etc, and the license of EDWinXP can be retrieved into a freshly formatted floppy disk/ USB flash drive.  
While uninstallation, inorder to backup the license, you may please insert the floppy in the floppy drive and from the EDWinXP - Uninstaller, click on uninstall, then a box will be popped up as shown below.


Then click OK so that the license can be retrieved in the floppy.

Q20. I am using EdWin XP ver 1.15 NC. Everything works alright until I try saving a job. All save options – Project Save, Project Save As and Project ASCII Save – remain dimmed not allowing me to use them.   What am I doing wrong?

We presume that your software was working fine till now.  
There may be several reasons for the malfunctioning of software.  
Check whether the saving option is not working after you have installed any other software.  
Check the software you installed and logged into the system in administrator mode, and not in any other mode for eg: user mode. EDWinXP should be installed in administrator mode for proper functioning.  
If the above suggestions couldnot solve your problem, After taking the backup from the EDWinXP folders → eg : LIB ,JOB etc, please retrive the license of EDWinXP into a floppy disk/ USB flash drive. You can retrieve the license using the format described below.  
While uninstallation, inorder to backup the license, you may please insert a newly formatted floppy in the floppy drive and from the EDWinXP uninstaller, click on the uninstall, then a box will display there as shown below.


Then click OK so that the license can be retrieved in the floppy.
  Then reinstall EDWinXP in administrative mode and activate the software.
Q21. By making a part I can create a symbol and a package, what I can also save. By saving the part, and open it later I can see only my package but not my symbol. What am I doing wrong? I was creating a  new coil with package.

You might not have assigned the symbol to the package correctly such that it is not appearing in the part editor.You please create the package outline in the component print layer. While in the part creation you have to specify the package details as name, type etc which is used for creating the part. For the addition of the symbol, Edit → Add Group and specify the symbol name. Then Edit → Edit pinout and enter the pins and save the Part. After editing the symbol or the package, save the symbol and package with check the box checked/ticked update in the part and on top of search sequence

Q22. I installed the software downloaded online but when I want to activate it with ID D0-2006331-369 and ID product 202143_224_1008_112448_198_9001526_265 no licence is found . I have a licence EDWIN XP v12 professional NC with licence disk serial no 1209184 and CD ROM, what do I have to make?


Please enter your Order ID in the page http://www.edwinxp.com/productdownload.aspx . After installing the software, click Activate Online button to activate your product. The ID is DO-2006331-369. Please enter this ID in the box and do the activation. (D and O are alphabets and others are numbers in the product ID.) The photograph shows that it is license disk of EDWinXP 1.20, so that EDWinXP 1.40 cannot be activated using this disk.

Q23. I am using EDWin32.I have a board with SMD pads that are connected to vias which are connected to power and ground planes generated using the copper pour tool. Is there any way to get hrf's generated for the vias connecting to the inner planes? Currently we don’t have the functionality to implement the hrf in vias.
Q24. I have recently purchased your EDWINXP software and have had early versions.I have had problems simple seting the PA text on schematic components to invisible. They always are visible no matter what I have tried. Please explain how I can make the PA (pin) text on the schematics to invisble.

It can be disabled from the Library Editor → Symbol tab → View → Disable PA text. Q25. What I need to know is how to make the pin out of the schematic component invisible when it is packed? I have tried everything to disable the pin numbers in the schematics even though in the entry properties I have made them invisible.

Please disable the automatic creation of Pinout in EDWinXP → System → Options → Packaging preferences → Pinout → Uncheck the “Generate Pinout text” so that the pinout text will not be displayed in the schematic while packaging.



Q26.At the moment I wil make a layout with only one layer but how must I configure the autorouter.It's look like  that I can only make a double layer or a multilayer, but to make a double layer print is at the moment to difficult for me. Can you help me for set up the autorouter?

For auto routing, the single layer can be set up Layout → Auto → Auto router → Arizona → File → Load Board to route from project (this will enables the board to be loaded to the workspace) → Parameter setup (first function tool) → Routing parameter settings (first option tool) → please disable/uncheck the option for signal lines and power lines in the layers except the layer needed for routing → Accept Select third function tool Auto routing routines → Second option tool Start Autorouter → Click on “Yes” on the dialog box Multipass routing → Select third option tool .Click on “Remove redundant vias” → Also Miter if necessary (F8). Or else this can be setup from the project setting EDWinXP project explorer → Project → Project Design rules → Routing layers and direction → Set the required used layer as vertical or horizontal alignment.

Q27. I did manage to download the rest of the file, but the SETUP file is not correct. It is not a .exe file! Any help will be welcome?

Please download the software from the location www.edwinxp.com/files/edwinxp140.zip Also please do the download to a location as for eg C:\ temp and unzip to another location as for eg: C:\ download After that, please run the setup.exe to commence the installation.

Q28. I have installed my EdwinXP again because I want to have the IEC library as default, but now wil my activation-code not work. When I ask for new activation-code the site says that I have activate my EdwinXP already, and now I have a really problem. Please can you help me? Is it posible to make a licensedisk or upgrade disk so that I have these problems in the future not anymore? I have also Edwin 1.6 and Edwin32 with all licenses.

EDWinXP will work even though it is set to IEC as default in the library.
The new activation code is as follows.
202359_174_16806563_348_58435_245_16810014_785_598_1730
Please paste this in the “Activation Code” and click OK
While uninstallation, inorder to backup the license, you may please insert a newly formatted floppy in the floppy drive and from the EDWinXP uninstaller, click on the uninstall, then a box will display there as shown below.


Then click OK so that the license can be retrieved in the floppy.

Q29. Hello, my EDWin XP is version 1:30; Revision: 20041202; nº series: 500912 distributed by VIPL  I have changed PC. Now I have a portable PC.  He/she doesn't have driver A:  How do I install the license? 

After installing EDWinXP in the evaluation mode, Please send us the product ID with full purchase details so that we may provide you the new activation code. The Product ID can be obtained from EDWinXP Main → Help  → Activate EDWinXP → Press the button Copy ID and paste to the mail.

Q30. I down loaded EDWinXP140 yesterday, It extracts Ok, but on trying to run setup I get a box with 'Invalid command line arguments. Unable to continue.'

Please unzip the contents of the zip file to a short file folder, for eg C:\temp. Then try to run the "Setup.exe" to commence the installation.

Q31. I have buy EdwinXP online and I have downloaded The software. My question at the moment is:How can I make a licence/upgradedisk from my old versions of edwin32 or edwin 1.6 to make a clomplete installing of edwinXP with all my licenses.

We presume that you have installed the copies of EDWin 32 or EDWin 1.6 in your system. For availing all the features of EDWinXP, please install EDWinXP1.40 as a fresh installation by running the "Setup.exe". and Activate the product.

Q32. what are the system requirements for EDWin XP 1.40? Will it run on a machine:
OS: Windows 98 SE
CPU: AMD Athlon XP 1.2GHz
RAM: 568MB
HDD: 12GB available


The memory management capacity of Windows 98 is comparatively lesser than other higher operating system for CAD based programs. Inorder to get better graphic display of the CAD programs, we recommend you to use higher operating system eventhough it works on Windows 98 SE. The other parameters will satisfy for the softwares working.

Q33. I’ve currently go someone interested in purchasing a copy of the product who has noted that the Motorola 68000 series are not in the product libraries. Could you please confirm whether these already exist or if we need to create this library for this client?

The component can be selected from the library as Library → Library Explorer → Parts → MOTMICR.PART → 68000. You can also browse through the library using Library Browser by entering the corresponding Part Name in the “Name” field.

Q34. I have just downloaded the upgrade to EdwinXp. When I run setup I get the following error message: invalid command line arguments, unable to continue. What do I do?

Please unzip the contents of the zip file to a short file folder for eg: C:\temp. Make note that it is not unzipped on to the Desktop or folders having space between them (for eg : Program files) . Then run the setup.exe inorder to install the software.

Q35. I have updated Edwin many times over the years.My old version 1.21 now thinks it’s a demo version

Please send us the product ID inorder to provide you the activation code.After installation of EDWinXP in evaluation mode, the Product ID can be obtained from EDWinXP Main → Help → Plug-in Licenses /Activate EDWinXP → Press the button Copy ID and paste to the mail.

Q36. Having recently upgraded to EDWin V1.4 I am once again face with the problem of the LIBRARY files that I have produced not working properly. I copied across the files from the remnants of V1.3's directory into theLIB folder of 1.4. I can see the library files when using V1.4 BUT whenI try to place a component it fails due to the symbol/package path not defined/missing. Please don't tell me that the components in the library I have generated over the last year or so needs to be regenerated in V1.4!

After adding the components from EDWinXP ver 1.30 to ver 1.40 in the LIB folder, please add them to the "Search Sequence" for loading the Parts. This can be accomplished from EDWinXP Main → Library → Library Explorer → View → Search sequence → Right Click → Select All. Follow this procedure for 'Symbol', 'Package' and 'Padstack' tabs so that the corresponding symbols, packages and padstacks are also added. Click on "Accept" to get the changes in effect.


Q37. I bought Edwin_xp_nc via internet down load at the beginning of January, to put on my laptop, as my old version of Edwin 1.52 would not work.I began to learn how to use the xp version, but not yet finished any drawings etc.Last week on starting the Edwin prog, it came up with some ‘module missing’ message, so I tried to re-install from my cd, Now I get lots of reasons why it wont work, and the previous activation code wont work , and from the website activation it says , act. Code already used, etc. etc. Any ideas how to overcome this , without making another purchase!!

If you are installed with the EDWinXP1.40 version ,please ensure that it is installed with Administrative privileges. After taking all the backup from the JOB,LIB folders,please uninstall the existing version and delete the existing installation folder. Again install EDWinXP in evaluation mode and send us the product ID along with full purchase details (if you have purchased EDWinXP, so that we may provide you the activation code. Product ID can be obtained from EDWinXP Main → Help → Plug-in Licenses /Activate EDWinXP → Press the button Copy ID.

Q38. i am new to edwin and now i am doing a project that generate gerber from autocad file using EdwinXP 1.30, the board are extremely simple, i just need the 1. board outline 2. NC drill layer, the holes 3. Copper track , without the need of solder mask and etc. What i want to ask is: 1. any requirement in autocad design should we follow to generate usable gerber file in Edwin? 2. What step involve in generating gerber from DXF file? Hope you all can help me, i am not technical student and this project make me headache. Hope your answer won't too technical for me. thank in advance.

The purpose of DXF import in EDWinXP is to bring in complicated mechanical features like board outline and cutouts that may be easier created in AutoCad. There are rules governing this import. Geometrics representing outline and cutouts have to be closed shapes. You have to create artwork file in the same way as from Gerber and then import it using Graphics imports. Subsequently reconstruct those categories that are possible to reconstruct. Graphics imported from Artwork Files may be directed to Graphic Import Categories in order to allow proper identification and interpretation during edition and reconstruction phases. Normally graphics defining traces, via or component pads are mixed in one import file. Categorized import enables to extract relevant types of graphic elements from Artwork Files and store them in dedicated places. The DXF files can be transferred to Artwork files by the following Fabrication manager → File → Gerber viewer setup → DXF preprocessor → then browse the DXF for conversion.  Check the ‘selection’ option in the “Gerber Preprocessor and viewer setup”. → Click on ‘Preprocess’ inorder to generate the Artwork files.



The process of graphic import can be executed as follows: Tools → graphic imports → import graphic item → Select  on Board outline → Right click on “Import  Artwork file” → Add artwork file



a. Board Outline to import graphic elements needed for reconstruction of PCB outline.
b. Board Cutouts to import graphic elements needed for reconstruction of cutouts in the PCB.
c. Silkscreen Comp. Side to import graphics element constituting silkscreen for Component (Top) side of the PCB. This category may be used as a template for reconstruction of components.
d. Thru-pads positions. Pad coordinates (flash D-codes) for Pin Mounted Devices may be imported from Artwork Files. These coordinates are graphically represented in this category and used as a template for reconstruction of PMD type of components. User can also assign hole diameters to thru-pads positions (with same size aperture) in order to reconstruct NC-Drill data.
e. SMD Pads Position Comp. Side. Pad coordinates (flash D-codes) of Surface Mounted Devices placed on Component (Top) side of the PCB may be imported Artwork Files.  These coordinates are graphically represented in this category and used as a template for reconstruction of SMD type of components. 
f. Thru-pads Padstacks. Graphic elements constituting PMD pads may be imported to this category. These elements may be edited for revision of artworks.
g. SMD Padstacks Comp. Side. Graphic elements constituting SMD pads located on Component (top) side of the board may be imported to this category. These elements may be edited for revision of artworks.
h. Via Positions. Pad coordinates (flash D-codes) are imported from Artwork Files. These coordinates are graphically represented in this category and used as a template for reconstruction of via holes. User can also assign hole diameters to via-hole positions (with same size aperture) in order to reconstruct NC-Drill data.
i. Via Padstacks. Graphic elements constituting PMD pads may be imported to this category and edited for revision of artworks.
j. Trace Master. Graphic elements constituting traces may be imported to this category and used for reconstruction of physical connection on the board.
k. Copper Planes Master. Graphic elements imported to this category are used to reconstruct copper planes and copper pour areas.
l. SMD Padstacks Solder Side. Graphic elements constituting SMD pads located on Solder (bottom) side of the board may be imported to this category. These elements may be edited for revision of artworks.
m. SMD Pads Position Solder. Side. Pad coordinates (flash D-codes) of Surface Mounted Devices placed on Solder (bottom) side of the board may be imported Artwork Files. These coordinates are graphically represented in this category and used as a template for reconstruction of SMD type of components. 
n. Silkscreen Solder Side to import graphics element constituting silkscreen for Solder (bottom) side of the board. This category may be used as a template for reconstruction of components.
o. Template Outlines. Graphic elements imported to this category may be used for reconstruction of template outlines.

The components, traces, etc can be recreated from Tools → graphic imports → Reconstruct from graphics , select on each item for recreating the Corresponding items can be recreated.

Q39. A customer has a problem with 3D presentation.
His proceed:- open library editor (project library)
- chosse part
- edit part
- edit package
- renumber pads
After renumbering the pads, the part in 3D view is now fixed at new pin 1 and it's displaced. So you have to move every fragment of the part to the new correct possition. Is there a possibility to place the part in one way (e.g. something like "Block move")?  Another thing is:After refreshing the project library three times (even there are no changes made), there are failures in the librefrshinglog. Only a few schematic symbols are found and no packages/parts. You also can't save a new part after this error message.

The 3D package can be shifted by copying the existing part and pasting it on the component outline and relocating it. This can be done from Library Editor → Edit → 3D viewer → Edit → Select all → Copy → Paste. Then delete the existing part. The new package can be relocated.

Q40. After refreshing the project library three times (even there are no changes made), there are failures in the librefrshinglog. Only a few schematic symbols are found and no packages/parts. You also can't save a new part after this error message.  I also made a live-update (update from 04. March 2006) but the problems still appears.

Please download and update the latest files from the link www.edwinxp.com/files/bugfix14032006.zip to the EDWinXP installation folder and check whether the error persists.

Q41. We use Edwin32 Ver 1.2 Rev 20000501 software for producing PCB designs and are very pleased with it. However we are encountering a problem when using the copper pour facility which I am sure is due to our not understanding the correct procedure for generating it! I have attached a copy of the file (zipped) in the hope you could have a look at what we are trying to do. The layout in question is in the hierachy called MAINHIER which has several copper pour areas. On the solder layer Edwin insists on inserting Heat Relief Pads around some of the holes. We do not want any HRf pads at all. I can temporarily remove them by switching them off using the 'Define Artworks' tool but they still appear in the Gerber view. As well as explaining how to do it I would be grateful it if you could actually fix it and e-mail the file back to me (the design needs to be with the PCB makers as soon as possible).

Please edit/delete the hrf items for the required pads whose HRF items are to be removed, from the library editor. Then save it to the library for the particular project and the existing package in the project is replaced with the new package. This process can be done for all the padstack that should be removed.

Q42. 1) Could you please tell me the whole process of making 4mm mounting hole’s in the PCB.
 2) Is there a way of showing the physical dimensions of the PCB
 3) Do you have various sizes of screw terminals with the 3d layout drawings
 Once again many thanks and best regards

1. The mounting hole can be made from the Library Editor → Padstack Editor → File new Padstack using wizard
2.Click on “New/Edit” tab.



3. Set hole diameter as 4.000mm.
4. Select the “show layer”  and give values for X-Dim and Y Dim as 4.000mm.
5. Click on “Make” . please ensure that the hole diameter and the layer sizes are having the same dimensions.



6. Click on “Select”.
7. Save the Padstack.
8. Select the Package tab, → Change padstack (9th functional tool) → select  padstack (1st option tool) → click on the workspace → Select the saved padstack which is stored .


9. Click on “Select” –(this makes the new padstack to be the one you created).
10. Then File → save Package, to a new file for package.
11 Then select the “Part editor” tab for creating special part for the mounting hole.
12.Please enter the name of the package that you have created in the “package details”  and give a part name and save this.
Also ensure that the part,package and padstack are selected in the “search sequence” in Library explorer-> view -> search sequence. Then if we load this part in the Layout editor,this will be appearing as a Mounting hole.
2. The dimensioning can be made from Fabrication manager → tools → dimensions → place dimension (2nd option tool) → first or second option tool used to place Y and X dimension respectively.
3. Currently we don’t have various sizes of screw terminals with the 3d layout drawings
Q43. I did install Edwin XP, the evaluation version, however there seems to be some sort of error ocurring that wnt allow me to use the application. A dialog box reading "access verification" comes up when i try to open the software, this contains an error thats reads "invalid text to decrypt" when i click on activate, nothing happens, do you have any ideas on what to do?

Please install the evaluation software with administrator power inorder to get it fully functional. If you send the Product ID we will provide you the extension code. The product ID can be invoked from Activate → Copy ID.

Q44. I have EdWinXP 1.40, updated with LiveUpdate with the latest fixes, license 33739. It seems however that the latest fixes made schematics go crazy.I fixe some issurs in schematics, and occationally EdWin redraws a number of wires or buses and connects them to lots of different wires. It looks in schematics that SPL0 connects to the data bus or something else. When this happens I often pich some completely different wire from the one that I am pointing to. Occationally when I save the project, EdWin shows some schematics DRC check report and wires become completely confused. This happens several times every day and makes EdWin impossible to work with.I supply you with the project I am working on. It doesn't happen every time, but you could try rerouting some wires/buses in Circuit MAINHIER, page MAINPAGE, then save the project.

Fix for Integrity check is now available.Please run Live update to get latest fixes for Integrity check. You can also get this from www.edwinxp.com/files/IntegrityTestFix.zip

Q45. Something strange happened :commands "Library Editor" and "EDSpice Symbol Editor" are now missing in the Tasks List of EdwinXP V1.40 / System /  Library. What must I do to make them visible again?

Please check the commands "Library Editor" and "EDSpice Symbol Editor" are present in the below of EDWinXP Main window (EDWinXP → Library → Library Editor/EDSpice Symbol Editor) by switching ON both “Task Lists” and “Task Tool bar”.

Q46. I have a problem with an edwin file and I hope that you can help me. I have attached a zip file with the edwin file and the component layer as we extracted it. Take a look at component IC1 and the area around the bottom 4 pads of this component. The copper area does not look correct.We produced this and now the customer is saying this is not the same as his layout. Unfortunatily our internal checks did not highlight the problem.The customer has sent in gerber files for us to remake the board and this area is correct. But on his new files there are a lot of tracking changes which means it is not the same board as he sent originally.Can you have a look and let me know what the problem is. Is it an error in his layout? or is it a gerber problem? We are using Edwin Xp V1.4 I dont know what version the customer uses. The PCB company I use to have my boards fabricated now offers a solder silkscreen option.Is there any way to generate a solder paste file using EdWinXP 1.20?

With solder paste files means Gerber artworks presenting spots where soldering paste has to be applied before spot soldering SMD pads to the board. You have to select one of the layers (ex A) as solder paste layer. Then add necessary item (rectangle) on this layer to pad stack for these pads in the packages. You have to select one of top layers (A-M) remembering that if you flips a component to the other side of the board then items from top layer are also flipped symmetrically to the bottom. Those on component layer are flipped to solder layer, from A to Z, from B to Y etc. “Symmetry line” for this flipping is located between layers M and N meaning that items from M layer flip to N. So it must be remembered that paste layer for components mounted on the bottom side of the board would need a separate layer for bottom solder paste. This will be handled automatically. If someone select ex A layer for top solder paste layer then (when component is flipped) solder paste layer item(s) in the pad stack will wind up on Z layer. It also means (in this case) that Z layer is reserved for bottom solder paste and should not be used for placing traces. To plot solder paste layer(s) properly on the Gerber, one should suppress plotting of PMD pads in the fabrication set ups for these layers. Since we do not have solder paste layer assigned by default, SMD packages have only solder mask and component layer items in the pad stacks. There are two different technologies for mounting SMD components. One is spot soldering where you need solder paste layer. The other is gluing with conductive glue. In this case you need a layer to store items that represent clicks of adhesive. This is equivalent to solder paste.

Q47. When I downloaded and installed the demo it says the activation period has expired. This happens immediately and has prevented any evaluation of the new version. Any ideas what I might be doing wrong? Thank you for your time in this matter.

This happened may be because the system time has changed automatically, ie the system clock may be weak and it changed the date.We have included 8051 kit and AVR kit to the newer EDWinXP 1.40 version such that it will be simulatable for a licensed user.

Q48. 1) When I create a Via in layout editor then draw a route to it, then I do an autocheck it comes up with error 4 for that via.
 2) is there a way of only viewing the tracks on component side only and visa versa?

1. The “error 4” is “Pad on trace/Item” which can be viewed from the Layout editor → View → Errors. 2. The tracks on the component side can be viewed from the Layout editor → View → Layout → Active Layers → Check only he component Layer to view the traces in that layer.

Q49. But how do I overcome the problem eg to get rid of the error 4. I place a pad and then draw a route to it. When I do a check error 4 comes up, I understand this but how do I rectify it?

This is  occurring because
i) the size of the pad will be a little larger and it is intersecting the trace
ii) the trace item will be having a larger width such that it gets overlapped with the vias.
The workaround is that you must reroute the trace apart from the vias or place the vias in a minimal clearance distance from the trace item.

Q50. I still get the three error messages during installation and EDWinXP still fails to run. I have used the register application to register the ocx's dll's and exe's, once again I see errors when the exe's are registered, same three that I see during installation Please, advise , why cant you ship a version that allows me to see the error messages that windows generates, by trapping the errors you are preventing me from seeing the root cause of the problem.

The unexpected error may occur due some version mismatch in the OLEAUT32.DLL and OLEPRO32.DLL s. Please send us the above dlls in you computer. Mean time you can also try this, take a copy of these dlls. Overwrite these dlls on your system with the same dlls from EDWINXP CD. And try installing EDWinXP.

Q51. I have a big problem.
It's the Half Term Holiday and I wanted to do some PCB work.I also wanted to upgrade some of the applications on my PC.I installed Microsoft Office XP, expensive, but good!The installation crashed, but a reinstall of Office XP fixed it.Now when I run EdWINXP140, I have no problem until I try to produce a Gerber then I see an active X error.SO I guessed that the Office installation must have overwritten something, so ( big mistake) I reinstalled EdWIN140 in new directory
hoping that would reinstall the active x and register the active x.Now I get the message unauthorised copy!!!!What must I do to remedy this???

This has happened because two installations are found in the system and one has installed over the other without having uninstalling the first.Please uninstall the existing version after taking the full backup of the files and backup the license to a floppy disk or a USB flash memory. Then install EDWinXP and activate with the license file that has backup.If it hasn't worked, please send us your product ID for providing you the new activation code with full purchase details.

Q52. I could not transfer the license activation to a floppy disk. The new installation was only a trial and the trial seems to have killed the license in the existing installation.I have now uninstalled BOTH installations of EdWIN XP 1.40.I have re installed the version 1.40 trial During installation I see three error messages all three say "Unexpected error: Quitting" After installation, running EdWINXP.exe from the installation directory results in some disk activity and then NOTHING, no error message, now application start-up, Nothing at all.I ran the update by executing e2kupdt, this ran an update application, found the updates and installed them successfully.Still when I run  EdWINXP.exe from the installation directory results in some disk activity and then NOTHING. What can be wrong, Please assist I have no working installation now.I have VB6 SP6 installed and updated, Office XP installed and updated. WinXp SP2 installed and updated.Please can you advise what should I do now? Please, How do I transfer the license to a Floppy disk?

Please unzip and run the attached exe file and install EDWinXP.For the installation, you must be in Administration mode; means the user must have administrative privileges. After the installation in the evaluation license try for activation .In your case since the license file has been corrupted, please send us the Product ID for providing you the activation code.For backup of the license file, while uninstalling EDWinXP, EDWinXP uninstaller → Uninstall → yes → when asked for "Enter license path",insert a freshly formatted floppy in the drive and click OK so that it will be retrieved into the floppy for another installation.

Q53. I was not sure of the exact procedure to use your clear application.I left the application installed and ran clear.I then used your uninstall to remove EdWIN I ran clear again.I then rebooted the machine I ran clear again I then installed EdWin During installation I still see three error message boxes. Each says "Unexpected error: Quitting" I close these during installation.Installation continues regardless of weather I close them or not.Still when I run  EdWINXP.exe from the installation directory results in some disk activity and then NOTHING.What am I to do?

Please do the following procedures
1. Take necessary backup from you EDWinXP folders from the LIB and JOB directory.
2. Uninstall EDWinXP.
3. Delete the EDWinXP installation folder from your computer.
4. Run clear.exe now.
5. Install EDWinXP again.

Q54. At this stage there is nothing to backup. I have my work on a separate disk.Uninstalled EDWinXP Deleted the installation directory Ran clear.exe Reinstalled EdWinXP Still get the three error message boxes "Unexpected Error; Quitting"Installation continues in the background Clicked ok on each of them.They disappear Installation completes Rebooted PC. When I run  EdWINXP.exe from the installation directory results in some disk activity and then NOTHING.

Please run "vbrun60sp6.exe" from "EDWinXP CD → Tools → Setup Directory". This error happens when some system files are corrupted.

Q55. On my EDWinXP disks there is only Vbrun60.exe NOT Vbrun60sp6.exe I have run this, but it has no effect of the problem.I should remind you that on this machine I already have VB6 pro SP6 installed ( and working)I have looked on both my EDWin XP cd and EDWin2000/XP cd there is no VBrun60sp6.exe I obtained the file VBrun60sp6.exe from: http://www.microsoft.com/downloads/details.aspx?familyid=7B9BA261-7A9C-4 3E7-9117-F673077FFB3C&displaylang=en I have run VBrun60sp6 update obtained form the Microsoft siteThis had not additional effect on the problem The Edwin application still will not run. I get no error messages. Nothing except some disk activity. The application closes without any screen activity at all.

The problem caused may be due to the corruption in EDWinXP CD. When you reinstalled the EDWinXP, due to the error in Installation setup, the setup was not completed. So we think that your EDWinXP CD is corrupted. So as an immediate solution you can download EDWinXP 1.40 from the following link
www.edwinxp.com/files/edwinxp140.zip
After downloading please do the following
1. Uninstall the previous Installation of EDWinXP from your computer.
2. Delete the EDWinXP folder.
3. Run the clear.exe which we sent you today.
4. Unzip the downloaded zip file to a temporary directory. Note that this directory name should not contain any spaces and this name should be sort as possible say "d:\temp".
5. Run setup.exe from EDWinXP140 Folder. Install evaluation.
6. When Installation is complete Run EDWinXP. This will popup a window for activation .Click on activate button and send us the Product ID.

Q56. I have been trying to eliminate unconnected copper fill areas using the automatic tool in Fabrication Manager.         When the PCB is inspected in the Gerber Viewer or an external Gerber tool, I get small, unconnected islands of copper as shown on the attached zipped bitmap.         I have tried smaller and larger square & rectangular tools with no improvement in accuracy. The polygon tool causes more problems, it can corrupt the Gerber output leaving shorts between other nets and the fill area. The algorithm also seemed to "miss" certain PCB features as well as use multiple small segments (< 0.001") instead of a stright line.         Changing the measurments from imperial to metric had no effect, I thought some of the errors were due to mechanical run-out between the two systems.         I have used the latest EdwinXp 1.40 Offline update with no change in behaviour.         Please advise any work-arounds to this problem.
EDwinXP 1.40
Rev. 20050615
S/N. 500938


After using the automatic tool, as a workaround, you can use the rectangular or polygonal tool for the removal of the isolated copper pour manually. Before performing the automatic removal, please fix the precision value to the maximum

57. I have upgrade the service pack of Gennary and I have this problems , when I move a component in PCB and I have enable the function Reroute or when I use auto connect net  function the programs generate a error. I send for you the file where you read the error ( BMP ) and the file that generate this error.

Please relocate the components which are placed outside boundary of the board.This message indicates that some components are outside of the board.For the auroroter to perform routing all the components should be inside the board.

Q58. I formatted my hard-disk and reinstalled my OS, and my activation code was not accepted by EDWin. And activation on line either !?

Please send the Purchase details of EDWinXP along with the Product ID, so that we may provide you the activation code. Product ID can be obtained from EDWinXP Main → Help → Plugin Licenses /Activate EDWinXP → Press the button Copy ID.

Q59. 1)Why I don't see the component in Library Explorer->View package when I don't select layer in Pcb Layout .
  2)Why CopyBlock don't work with bus.
  3)Why the utility Airgap for Layer abjects work on both layer ( I change the airgap SMD pads on sold.layer and I see that the change is apply on both layer).  
4)I open the EditPackage and I enable View->Toolbar->Sizes , I close the EditPackage , I open the EditPackage and the toolbar sizes there isn't.  
    The computer where EdwinXP is installed it doesn't have access to internet , when you fix the problems can you send for me the file or  internet link  with update.

1. When disabling all the layers in the PCB Layout or in the Library Editor → Package Editor, none of the layers is selected for viewing purpose. So it has no layers to display in the Library Explorer → View Package, hence no package is visible. 2. The copy property of the buses is set as so because the properties of it could not be mapped with multiple entities of buses in a same project. We are looking on to this issue and the suggestion has passed over to the R & D team. It will be available with the next release. 3. The airgaps can be set for each layers. 4. We couldn’t reproduce this. Please update with latest files. The offline update will be released soon

Q60. 1) If I want to connect to our EdWinXP licence server over internet, how do I do? The firewall at the licence server detects a TCPSMB connection, so I got a connection from my client. But the client only gets "Server Not Valid". Which ports are used by the licence server?
2) If I create a copper pour area, like the GND plane, how do I create empty areas in that plane? I want to make areas without copper on my GND plane.

1) The EDWinXP license manager is intended to activate and to connect the clients in a intranet environment (LAN). After installing the software in a server, the clients has to log on the server, from Start → Run → \\computername of the client machine. Then type the name of the server in the activate EDWinXP so that the client communicates with the server and it gets activated.
2) The empty areas can be created by using the Copper relieve option in the Fabrication Manager. After creating the Artwork files, select the net for which the copper pour area is drawn, Select View → Artwork → Copper relieve edit view.

Q61. We have a problem by copying busses, see bus-test.epb. I´ve routed a bus named D0-D7 and added six nets UN1 .. UN6. I´ve placed the net names and bus member numbers, see upper left drawing.After block copy (no F3 pressed), I get the upper right drawing.The nets are merged.The bus line is not visible. The bus member numbers are switched to net names. With F3 set, I get the lower left drawing. There is no difference to the upper right.What is wrong?

The copy property of the buses is set as so because the properties of it could not be mapped with multiple entities of buses in a same project. We are looking on to this and the suggestion has passed over to the R & D team. It will be available with the next release.

Q62. A problem has somehow cropped up with Edwin XP 1.4NC.  In library explorer when selecting a part it comes up with Cant load part: suitable symbol/package: for part cannot be found  Why is this ? as it always was there.  This seems to be doing it for most of parts from the library

Please check the Library Explorer → View → Search Sequence → Select the Part / Symbol / Package / Padstack tabs and → Right Click and “Select All” for all the tabs → Accept.

Q63. I am an old user of your Edwin product. I downloaded the demo/trial for EdwinXP 1.4 but it wont run on my machine. Information I got from the machine manufacturer indicates that v 1.3 should run. Is there a chance of me getting the demo for edwinxp v1.3 to check out. I need to make sure before I place an order

EDWinXP 1.40 runs on all Windows operating systems above Windows 98.Please specify the operating system and machine details such as
Operating System Type:
Operating System Service Pack:
Operating System Default Language:
Total Physical Memory/ Free disk space: etc.
The software can be evaluated from the link www.edwinxp.com/files/edwinxp140.zip

Q64. Potencial customer asks us about compatability of Edwin's VHDL code(edn files) with Xilinx environment. Is it possible to to debug files in Webpack ICE? Have you checked Xilinx converter code's compatability with Spartan, CoolRunner families. I have not ...

The code in edn file is compatible for the Xilinx software. Please refer to the attached pdf file in the zip. Refer page 35.

Q65. I have see that is impossible to edit and save one symbol or package in the PROJECT LIBRARY whitout saving them in anoter library and then change the componet in the project. I don't know why? I think that this function is very important & helpfull in whitch case is not so important change the components in library but only change the components in the project.  Can You suggest to me what's the best & short way for make this operation?

The components loaded in the schematic are listed in the Project Library. Inorder to change the symbol or package, you can use this method.
EDWin XP → Library → Library Explorer → Part Project Library → Right click on the Part whose package has to be edited → Edit Part → Edit → Edit Package "xxx" → After making necessary changes → File → Update Package to Part → Goto Part tab → File → Update Part to Project Library. If you want, you may save the changed Package and Part in your library using File → Save Part/ Package.
NB: You cannot add or delete entries to any used package or symbols.

Q66. I reminded Jivan about sending the evaluation board to you, but in the meantime the lot that was produced is again sold out. We are producing the next lot now, but it can become available only next week. So we will send it next week. I am sorry for the delay. Along with the board, I will also send the CD with evaluation software. Meanwhile, we received an enquiry from a College. It is not an Engineering College, but Science College. They do not need PCB designing but they want Schematic entry and simulation. e.g. he asked that they want to enter a schematic with some OpAmps (an amplifier circuit). Then they want to simulate the circuit i.e. simulate some input to it and observe the output. Then change some component values and again observe what difference it makes. Is it possible using Edwin? Also, since it is Science College, they do not have funds. He asked about prices and he thinks the price is too high for him. He compared the price with another software - he called it "Tina" or something like that. I don't know what is the price of Tina. Are you aware of it? Also please inform us whether the simulation (as mentioned above) is possible.

The simulation of OPAMP is possible in EDWinXP so that the user can create the circuits as Amplifiers, Oscillators (eg: Wein Bridge, RC phase shift) etc. The simulation function of OPAMP is embedded as subcircuit in EDSpice Simulator and as code model in Mixed mode Simulator.

Q67. How does "Horizontal NET/BUS page links" work?

The horizontal page link is used to connect the same nets in two different pages in a horizontal mode,which acts as a offpage connector. The Schematic → Connection → Edit Connection → Place Net-Page links.

Q68. In what is new I found this sentence :
  "Mixed Mode simulation models may be assigned individually to components, hence overriding current model assignment to symbols. Component specific simulation models may be assigned to block diagram elements." How to do this .

Here the elements are considered as Parts and the model assignment can be done for the components (Parts, i.e. component specific) rather than symbol in the library.For eg : if a functionality is given to 2NAND gate and another functionality is assigned to its coreesponding Part ie 7400, then the model function of 7400 overrides the symbol’s functionality . A block created with the help of the Library editor can be given the parameters of a simulation model to function it as a component. Earlier the symbols can only be assigned with the corresponding model.

Q69. A customer sent us the attached library. It's an old library from a earlyer version of EDwin (don't know the version). Some parts (e.g. 1N4448) can't be loaded, other parts (e.g. _RAM8_32) can be loaded in the schematics/layout. His current EDWin-version is XP 1.40. In the attached picture you can see the error message. Could you please tackle the problem and tell us what to do in the future with such problems?

The library should be assigned with the simulation parameter for the particular component to get loaded in the schematic / layout. This can be achieved from Library editor → Part edit the component 1N4448 → edit → edit symbol → Properties → symbol properties → assign the corresponding parameter and select the edit entry attributes for assigning the simulation function. And from the library → field editor → select your, symbol, package, padstack, part library respectively and right click → select Read System Values. Then again after processing right click and select Update symbol/ package/ padstack/ Part → All. And save the part files in your coresponding libaries

Q70. I’m using EdwinXP version 1.30. Isn’t it possible to have a Font Size smaller than 0.06” on my layout editor? Because this is too big for my PCB. And how can I change the font size/style of a component name?

The text size can be altered in the EDWinXP → System → Options → Layout → Text to the required value.

Q71. I use EdwinXP Pro 1.30.  There is an option (View>Long Cursor) to set the cursor with long lines, that eases alignment etc. I have to reselect the option each time I start Edwin. Where can I set or save this so I don't have to select this each time again?

If the long cursor option is selected for a project, it will be set for it and it will remain for the same instance of EDWinXP and for each new instances the option has to be enabled

Q72. I'm Tsubota who belong to Unicraft.Please asks for inspection about library conversion of OPUSER XP.when a customer converted these library, OPAMP does not work.I tried setting with an filededitor, but it does not go well. please check these library.

It seems that the files doesnot contain any OPAMP components.

Q73. I am evaluating Edwin 1.20 and have a problem. When I´m creating a component and number it´s entrypoints-sometimes the entry text turns 90 degrees and also affects the entry (also turns it) next to the one I´m working with (they seems to interact when they should´nt) I attach a file in this mail, of the component which should describe the problem. Here I want the entry #16´s text to be vertical. When I turn it vertical , #17 gets horisontal and vice versa. I want both to be vertical-why do they affect each other? Please tell me how to solve it.

We have checked the symbol and found that the pins/entries are not placed in the grid lines . The grid should be set to ‘Line’ and of value .1000” and snap of value .0500” for creating the symbol. If these parameters were set, the entries would have been correctly arranged. If you find it difficulty to create, you may request to our Library support through our website which may take a delay

Q74. I have a patch antenna design created by a third party. The antenna is basically a copper pour area which could be applied to either the component or solder side.   I would like to re-use this by packaging it as a part. I will use a SMT pad to provide a connection point for traces.   Can I import this design into the package editor? The Gerber and DXF files for the antenna are attached.   If not, can you describe how I to import the DXF file using the fabrication manager to either the component or solder layers? I have tried using your online help, but the import produces traces only and does not fill the area. Also the scaling is incorrect (the square part of the patch is 1100 mils each side).

Open project explorer → select from the task list and open fabrication manager. From Tools → select Gerber view → to get Gerber preprocessor and viewer set up  From the top select DXF Preprocessor → select the DXF files and select preprocess to get the artwork files.



From the top artwork viewer set up → select browse artwork → select the .art files → select view all → close to view the artwork


Q75. By making a part I can create a symbol and a package, what I can also save. By saving the part, and open it later I can see only my package but not my symbol. What am I doing wrong? I was creating a  new coil with package.  Please can you help me?

You might not have assigned the symbol to the package correctly such that it is not appearing in the part editor.You please create the package outline in the component print layer. While in the part creation you have to specify the package details as name, type etc which is used for creating the part. For the addition of the symbol, Edit → Add Group and specify the symbol name. Then Edit → Edit pinout and enter the pins and save the Part. After editing the symbol or the package, save the symbol and package with check the box checked/ticked update in the part and on top of search sequence.

Q76. I have downloaded the file to upgrade my previous version of EDWin XP Professionnal NC (v1.10 revision date : 2001-10-25 Sn : 9908048) to v1.40 Professionnal NC.  With my previous version of EDWin XP I have all options: Mixedmode and EDSpice simulator, thermal and field analyzer.  But when i install the downloaded upgrade the thermal analyzer has been disappearing!  Is the thermal analyzer accessible of another menu as both simulators now? See my screen copy of EDWin for my question.

The Mixedmode and EDSpice simulator are integrated in the schematic editor, thermal and Electromagnetic analyzer/ field analyzer are included in the Board analyzers 

Q77. I have Edwin XP/2000, Version 1.1, Revision date: 2001-10-25. Should I be able to run it on a PC with XP and Service PK2. Do you have any service packs, or updates.

We suppose that it will run under your work environment.