Schematic Capture

Q1. How can I make my working sheet large enough to draw a big schematic?

The page size may be redefined using the tool from Tools à Page format menu item. Right click on the workspace and select the tool Define Page. You will get a window where the new page size may be selected. Otherwise you may draw the rest of your schematic in a new page by defining a new page from File ? New Page. The maximum size for a page that is acceptable is 4 x 4 meters and the maximum number of pages that can be used in the Schematic Editor is 99 pages.

Q2. In Schematic Editor, after a circuit is drawn, we autopackage. Can you explain what is actually taking place in autopackaging and why?

The autopackaging utility allows to perform the automatic packaging of all unpacked components and it assigns the first free number to the last placed components belonging to the same group. The component name prefixes from Part descriptions are used to automatically generate component names.
        When you actually autopackage, system extracts the package assigned to the part at the time of creation. This is how it displays the respective package facilitating front annotation.
Note: After Autopackaging if any components are deleted, then using Compact Project Library from EDWin XP/2000 task, compact the project library to avoid irregular numbering of components or corruption of the project.

Q3. EDWinXP concept of nets and wires

Net is a collection of nodes that are electrically connected together. A wire is merely a visual representation of the corresponding net description. The creation of a wire automatically results in the creation of the corresponding Net. Further, the deletion of a wire removes only the wire but does not remove the Net whereas the deletion of a net removes ALL the associated wires. The deletion of a node in the net removes the corresponding connection in the net and removes the associated WIRE SEGMENT/ TRACE SEGMENT also.

It is possible to delete a wire and the corresponding net connection together by the following procedure. From the Schematics Editor/ Layout Editor window select Tools -> Nets. Select the tool     Delete a Node (shortcut *NN) from the toolbar. Click on the appropriate node. A confirmation box pops up asking to confirm the delete operation. Select Yes to delete the node. This will delete the associated WIRE SEGMENT/ TRACE SEGMENT also.

Q4. How do you print the schematic hierarchy contents?

To print the schematic hierarchies select the specific schematic hierarchy from the list of hierarchies and select Schematic Editor. Then select File-> Print Page to print the schematic hierarchies.

Q5.How do you change the thickness of wires?

The thickness of wires & buses can be changed even after routing.

1. Invoke Options ? Sizes ? Schematic ? Bus/Wire from the task EDWinXP in the Project Explorer.

2. In the edit boxes provided for bus and wire line width, change the value.
Now to effect this change as the default setting, select the “Save & Exit” from the dropdown button before exiting from this window.

Note: If this change is just for the current project, then click the APPLY button and exit.

Q6. When I use "redraw on component" in Schematic, an error-message "component not found" appears although the component is apparently there in the schematic.

When you redraw a component in Schematic, specify the group number of the symbol on which the zooming operation is to be done, i.e. to zoom on 7474,1 that is packaged as IC4 in the schematic. Enter the name as IC4/1 in the input box that pops up when "Redraw on Component" is selected. On the other hand when redraw on component is done in the Layout, only the name IC4 is to be entered. Enter the component name in the format given in the input box that pops up when Redraw is selected.


Q7. About Merging and Splitting of Nets: I am not able to split and also end up in merging the nets which I don’t want to?

Splitting nets is a very simple process in EDWin. Select the tool Split Nets from the Wire/Bus toolbar. Click on the wire, the entire net gets selected. Click once again on the same wire, this pops up a window, enter a new net name (system automatically inserts the first free number) and check “Named ” in the window. Accept the new net name and verify using the tool Wire/ Bus Property.

But the system won’t allow splitting a net that has only a single branch as shown in Figure - 1.

Figure – 1    Figure -2
To split such a net, you have to delete a wire segment so that two or more branches exist in the net as shown in Figure - 2. Now select any node in the net and the system prompts to select the next node in that net which is to be splitted.
To merge, invoke the tool Merge Nets. Select the net you want to merge and click on the other net. A confirmation prompts. Now click YES to merge two nets into one.

Q8. I made the schematic diagrams and the layouts for an audio pre-amplifier and amplifier in 2 different projects. Is it possible to merge the two diagrams to create one single schematic diagram and layout?

You cannot make any link between two projects in EDWinXP. You can use Block Save / Block Load facility to combine two projects. Open one project and Block save its layout and open the second project and Block Load the first layout. You should make necessary net /trace connection between two layout parts if required. Block Save/ Load tool is available in Tools à Block Edit for both Layout Editor and Schematic Editor.

Q9. I created three buses with different names A, B and C. Then I suddenly discover that two of the buses should have the same name. Is there any easy way to change bus name without deleting it and rewriting it again, because when I try to rename C as B, the system says that B already exists?

You can' t merge two buses which are already created. EDWin will not allow this. The only possible way is to give similar names at the time of bus creation. For e.g.: create one Bus and give names as B and create another bus and give again B. But after creation you can't merge it.

Q10. I tried to copy a schematic to a Microsoft word software, (zoom1: 1), and I got half of the picture in my word document.

When I copied the schematic to the clipboard (zoom 2:1) to Microsoft word document, I got a very unreadable picture in the word document. Please tell me, is it a different way to copy schematic to word document and still to read the schematic in the word document.
You can use File à Copy Screen to Clipboard "Ctrl+C" command to copy the capture screen. It will only copy the currently viewing part of the diagram (work area). Then paste it to bitmap editor and load this bitmap to word document. Or you can directly paste it to the Word document without loading to the bitmap editor. You can also use basic Windows operation such as "Print Screen" / "Alt+ Print Screen" to copy full screen/ highlighted window handle.

Q11. I cannot find a method of searching for an item. E.g. a resistor. I would like to search for, say R234 and have it highlighted in some manner in the schematic and the layout (perhaps elsewhere too) - is there a way to do this?

Objects on the workspace can be easily found out using CTRL+F combination key. This pops up a dialog where each of the object is displayed in different tabs. Click on the any object and select its name by browsing and double click on it to redraw it on the workspace.

Q12. How do I search for a particular net in a project?

If you want to search a particular net from the project, select the tool Net property from the Nets Toolbar (Tools->Nets) and click on the free workspace and the system prompts you to enter the net for search. Give the exact net name to highlight it on the page/board as well as to open up its property window. Use CTRL+F to find.
Look into Q11.

Q13. I want to group components of same type like resistors to one side of the board. I tried to do in EDWin, but always end up in Placement pattern cannot be completed.

You can set the values for components in Schematic Editor module using the tool Add text/ value.

Ø    Select Tools/Components from the menu or click Components in the Tools Toolbar.

Ø    Select the tool Add Text /Change Value and click its option tool Add change/ value.

Ø    Just click on the component, a text box pops up, where you may enter the value and Accept it.

Q14: Can Edwin rotate components in 10 ° steps?

EDWin allows you to rotate a component at any angle you want. Just enter the angle of rotation which you want in the dropdown ‘Angular Snap’ (Standard Toolbar) and then rotate the component. Minimum angle is 0.01° or specify the angle of rotation in the property window.

Q15: How can I stop the Bus member number sliding, when I delete a net, that is bus connected with a defined bus number? I wish that the other nets in bus hold their previously defined bus member numbers

If you are deleting the whole net which is connected to the bus by selecting the tool     Delete whole net, then on redrawing the circuit the bus member number also gets renumbered. This is because on deleting a net, the part once again gets repacked and it renumbers the bus members also.

More on Bus member number

Bus member number allows to group nets having the same bus member number, So it is advisable to have default numbers (0,1,2...). If the default bus member number (e.g. 0) is to be changed, then select the tool Add Net/ Bus Labels from the Wire/Bus Editing toolbar and click on the bus member number. In the window, enter the required name (D0) and click O.K. Now click on all the bus member number having the same bus member number (0) and assign D0.

Swapping refers to interchanging the pins of components. If Swap Level is set to -1, it will not allow the pin to be swapped. If it is set to 1 or any positive number, this means that the pin can be swapped with any other pin having the same swap level. For e.g.: the input pins of NAND may have their swap level set to 1 since they may be swapped. But the output pin of NAND should have this swap level set to -1. If you want to view pinout after packaging, you can set the Visible Pinout option (in the window where we edit entry attributes) i.e. it decides whether pinout label should be displayed after packaging.

Edit the symbol in the Library editor and check PA Texts from View menu. Position the PA Text and select the "Edit Entry Attributes" tool. Now click on each entry and check the "Visible Pinout
" check box. This will display the pin numbers in the Schematic after the component is packaged.

See that in the Packaging Preferences, the option to view the pinout is checked. To check this option, select Options ->Packaging Preferences ->Pinout from the task EDWinXP in the Project Explorer.

Now to effect this change as the default setting, select the “Save & Exit” from the dropdown button before exiting from this window.

Note: If this change is just for the current project, then click the APPLY button and exit.

This could have happened in the following way:

For e.g.: LF147 contains four schematic symbols OPAMP, OPAMPA, OPAMPA, OPAMPA. To load the part LF147, open the library browser and search for the component LF147. When you drag and drop this component on to the schematic, you get another input box with a drop down list. Select the symbol OPAMP. When ACCEPT is clicked OPAMP is loaded. If this step is repeated again, another OPAMP symbol will be loaded. Now packaging the symbols will load two ICs of device LF147 in the layout. This is because device LF147 contains only 1 OPAMP. On the other hand, if you select OPAMPA from the symbol dropdown list while loading the part LF147, and then package, you will get only one IC in the layout since a single LF147 contains OPAMP and OPAMPA. The function tool Repack allows repackaging an already packaged component. Packaging of a component is done according to the setting in the EDWin project Explorer Options/ Packaging Preferences. The three settings in the Preferences
for packaging are Component name, Description and Pinout details. Any or all of these can be set or removed. If you select a packaged component, change the default settings of Packaging Preferences and try to package it again, an error message appears saying “This component is already packaged”. So to package the component with the new details use Repack tool.

If you have any prerouted traces, and you are switching to autoroute with these prerouted traces. Autorouter will delete all this by default. If you don’t want to delete this traces, then you should uncheck the options, which pops up when you invoke Autorouter.
They are:
Delete wires not connected to node
Delete wires connected to single node
Delete wires with non orthogonal segment

Uncheck all these options and now try to route this. Now it will not delete your buses and prerouted traces if any.

There is no tool provided for viewing the unrouted traces. But you can check this from the menu Info->General -> Nets after existing from Autorouter window. The Net Map window will list out all the nets exist in that particular project and the right side window will show the components exist in the selected net. For e.g: first select one net from the left side box" Items". If the net is properly connected the column ‘Status’ will show "Connected", means wire connected. Now find the schematic component associated to this net and connect wire to it manually.

We have an option in EDWinXP called Project Properties, in which Wire thickness, Symbol outline etc. by value or percentage. Increase these values according to your requirement and try printing.

Thanks to EDWin’s new Windows like features, this is possible in different ways.
a) Bullet/ Select the components which have to be packed (Ctrl + Click) à Right Click à Properties à Schematic Component à Select “Schematic Components”à Right click à Pack. Similarly, it is possible to Unpack and Repack.
b) Info à General à Choose Tab “Sch. Components” à Select the components to be packed (Ctrl + Click for non consecutive selection and Shift + Click for consecutive selection) à Right Click à Properties à Select “Schematic Components à Right click à Pack.

Library Explorer -> Alt + Drag Drop the part to Schematic/Layout component whose reference has to be changed. Alternatively, bullet the component and change the name of the part in the property window.
The same applies to Layout Editor.

Make sure the part library is submitted to the search sequence. Library Explorer à View à Search Sequence