Q6. When connecting a trace on the component side to a component with legs, the trace is connected to the component layer pad. Is this pad connected to the solder layer pad on the other side of the board? Or should one put in a via.
Q8.With Edwin and View à Layout à True size on, I appear to be unable to select a via which has already been place on the PCB. If I turn true size off then selecting a via on the layout is no problem.
Q14.I am having difficulties with the manual routing of traces in the Layout portion of Edwin. Enforcing orthogonal traces seems to be quite difficult. When switching into the Router it complaints of non-orthogonal traces. Am I missing something or is there some secret?
Q17.Some parts of my layout have to be routed manually, because there are high voltage sections on the design. Therefore it should be possible to 'tell' the Autorouter, that some regions of the PCB should not be routed.
Q19.I downloaded your sample library of the month and EDWin does not recognize it to load. I go to File/Open project and only *.EPB files are shown. When I specify the *.edb files it says can not load project. Are these files not compatible or am I doing something wrong?
Q1:After Schematic Editor, I opened the Layout editor, but
Packages does not appear. In Layout editor I dont see anything, only PCB frame.
After placing the components in Schematic Editor, they have to be packed. Only then will the footprint of parts will become visible in Layout editor, and they will be all positioned at the Board Datum. Relocate one by one (use redraw to make the next part visible) on the board or do Autoplacing.
Q2: How can I add text outside the board outline, indicating layer of the particular artwork, to my PCB design?
Create the required text as follows: Select Layout Editor-> Tools-> Texts-> Create Text. Click on the workspace. Type the text in the window that pops up and place it outside the board outline. (before creating the text, you may select its placement layer using the menu, Layer). The placement layer of an already created text may be changed using the tool Text Property from the toolbar. Now, in the Fabrication Manager module, generate the GBR file for the particular layer. Preprocess the GBR file to an artwork file. Now in Tools-> Gerber view you may view the text created placed above the board. In case a text string, which is not needed in the artwork, but is required to appear only on the screen, use Tools-> Notes in the Fabrication Manager module
Q3: Can we have a utility that hides the comp. Name in the module layout?
Of course. Select Tools-->Component -> and select the function tool "On/ Off Component name" and click on the component name which you want to hide. To get the name back, you have to click on the component.
Q4: Will a click on an incomplete trace result in a finish of that trace (as it should) or does it make a new trace with all the possible errors involved?
EDWin will assume a click on an incomplete trace as a new trace element. Clicking on the incomplete trace with the tool Allow T-Connections enabled will create trace element as the part of the same NET. Without selecting this option, it will create a new NET.
Q5: What are branches?
Branches refer to the portions of a single net that is physically connected with two or more parts.
Q6: When connecting a trace on the component side to a component with legs, the trace is connected to the component layer pad. Is this pad connected to the solder layer pad on the other side of the board? Or should one put in a via.
For a through hole components (PMD) pads will be in all layers and it is not necessary to connect to solder layer or through via pad.
Q7: Can you define Channel Width .How can I do the clearance check? If I have a 10 mil trace, and a channel width of 25 mils, what will be clearance to the next trace?
Channel width of a trace simply means that the system should reserve an area for that trace. i.e., if you have a 10 mil trace, and a channel width of 25 mils, 12.5 mils (25/2) will be reserved on either side of the trace.i.e. A total of 12.5+10+12.5 mils will be reserved for the trace.
Q8: With Edwin and View à Layout à True size on, I appear to be unable to select a via which has already been place on the PCB. If I turn true size off then selecting a via on the layout is no problem.
To select a via, you have to click on it's periphery, whether true size is ON or OFF.
Q9: How can I locate the center of the padstack for the purpose of routing? Can I use a full screen cross on the cursor?
You can use full screen cursor. Press Shift+Z to toggle between Long/ Short Crosshair cursors while performing an operation such as Relocate, Repeat, etc. To confirm the selection of the pad is to use F3 option tool while routing. This option allows only pin to pin routing. To continue with free routing, disable F3 while routing and enable F3 at the time of connecting to the pad.
Q10: How can you display the ratsnest of the net being currently routed?
The tool 'Route Trace' in the Layout Editor has an option 'Display nodes' (F8). If this option is selected while routing, the nodes of the currently routed net will be marked. A better way to identify the unconnected nodes of the trace being routed is to check the options Preferences-> Guidelines [Next unconnected node]. Preferences-> Guidelines [Net] shows the ratsnest for the net being routed.
Q11: I made a square copper area on the component layer, just for cooling purposes. But I only see the outlines the area is not filled. Could you please help me with my problem?
Create the copper area along with 'Filled item' tool selected. Make the View->Layout->True size ON to get the filled effect.
Note: Filled option is available only for regular shapes. For irregular shapes, use copper pour area.
Q12: What does AGAP do and what is it for?
Agap is the minimum electrical insulation required for a trace, pad or for a copper item. Only the traces currently being routed take the Agap value that has been set in the Agap combo box. All other traces continue to take the default Agap setting. In order to change the default setting of Agap to the one desired, select Options from EDWin Project Explorer and choose Sizes-> Layout->Airgap. Here, the airgap widths for trace segments, Round & square pads can be set.
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.
Q13: I have a board with several hundred pads and I want to change their size graphically. Can you please tell me how to do this without deleting and recreating them all?
For this you have to make changes in Packages. Select a Package to edit in Library editor. For changing the padstacks select the tool "change padstack" (last tool) and its option tool F1 or F2. Option tool F1 is used to select an existing padstack in any padstack library. After selecting F1 click on the work area, will pop up a window "select padstack". Click on the required padstack and click on Select button. Then click on the required padstack in Package to be change it to a new one.
Note: Block select for multiple replacement with new padstack.
Option tool F2 is used for create a new one. Click on the work area to pop up a property window "Create padstack". Enter the values and click on Accept. Then click on the required padstack in Package to change it to a new one.
Q14: I am having difficulties with the manual routing of traces in the Layout portion of Edwin. Enforcing orthogonal traces seems to be quite difficult. When switching into the Router it complaints of non-orthogonal traces. Am I missing something or is there some secret?
Auto router deletes all prerouted non orthogonal traces (traces having bending points other than in 90°). So route all necessary traces in 90° and load to the autorouter.
Q15: Does the software allow thermal pads for SMD and PMD (through hole)?
It is not possible to create thermal pads for SMD. For PMD (through hole) the system will automatically generate HRF (thermal pads). Actually there is no need of HRF items in SMD. If you are so specific about it you can create it manually. See Tutorial for how to create padstacks.
Q16: I am trying to import a dxf board outline but it keeps hanging with the busy light on. Why?
There are certain conditions that must be kept in mind before importing .DXF files.
Some of the conditions are:
1) Issues an error message Board outline is not closed at x,y, if the created Board outline does not enclose an area.
2) Accepts board outline created only in single layer from AutoCAD.
3) Allows importing board outline created only with arcs, lines and polylines
4) Does not consider board outline created with double lines and arcs (i.e. Multiple lines created in AutoCAD enclosing an area) using a single tool as shown below though it encloses an area.
5) Relaxes board outline to be created upto a maximum of 32000/ 32000 mils or 32/ 32
6) Never accepts board outline created, having graphic items drawn unknowingly or having cut-outs that does not constitute the board outline.
7) Also allows defining the airgap and Line Size values for the board outline before or after importing. Add point and Delete last buttons gets disabled after importing the .DXF file. Editing may be done to the imported board outline in the Layout module and saves it in EDWin32.
8) Issues an error message while importing circular board outline from AutoCAD because EDWin32 consumes less time in creating circular boards rather than importing from AutoCAD.
May be the dxf file which you are trying to import may be overriding any of these conditions.
Q17: Some parts of my layout have to be routed manually, because there are high voltage sections on the design. Therefore it should be possible to 'tell' the Autorouter, that some regions of the PCB should not be routed.
If you just want to isolate your board from autorouting then do as follows:
Select Tools->Copper from Layout and create Copper blocks in the required shape (Create Copper Graphic item->Create circle along with FILLED Item" tool ON) and place it on the board in the area through which routing shouldn't be done. Remember that if you want to avoid Component layer routing, then you have to place Copper block on Comp. Layer. This is same for other layers also. And then execute autorouting. You can view that the router will not route over the placed copper area. While placing copper if you want, you can switch ON the F7 tool and the created copper item will not get connected to any net.
Q18: Can I create a copper pour area that is Hatched?
Please do the following steps inorder to produce hatches over copper item.
1) Create copper item using circle or rectangle.
2) Next enable the function tool "Hatch Copper" and choose the option tool F3 i.e., "Select items" tool and select the copper items that are to be hatched.
3) After finishing the selection enable the option "Execute Hatching" (F1) tool. Now click on the working area to invoke a dialog box in which the hatch pitch may be entered. Here we have entered 0.1".
4) Click OK and return to the workspace. If you have enabled the option F2 then hatching will be performed at 90°. If you turn off the True size view you can view the hatches.
Q19: I downloaded your sample library of the month and EDWin does not recognize it to load. I go to File/Open project and only *.EPB files are shown. When I specify the *.edb files it says can not load project. Are these files not compatible or am I doing something wrong?
EDWin 32-bit projects cannot load *.EDB files which are created for EDWin 16 bit version. To load this, first you have to convert those *.EDB files to *.EPB format. You can do this using Conversion manager utility which resides under the task EDWinXP in the project explorer. Run this program and choose the tab "Database conversion" and select those 16-bit databases and double click on the name. And start conversion and save it to *.EPB format. Now you will be able to load this in EDWin. The similar procedure should be done for all the 16-bit library symbols also. This you can perform by choosing the tab "Library conversion".
Q20: In Layout Design, is it possible to move a block of components on only one layer while still have all other layers visible?
Select Tools->Block edit, "Relocate by Vector" function tool and select the F3 option tool. Select components in block and enclose the components to be relocated by vector in a block. When the block selection is over, select the option "End Selection"(F1). Now the pin about which relocation is required is to be clicked. It gets marked with a rectangle. Now move the cursor in the desired direction and to the desired extent so that the selected block gets relocated relative to this direction. On clicking the mouse, the block gets relocated.
Q21: How can I place Pads on the PCB in the layout editor?
EDWin does not permit placing pads on the PCB. Instead, it provides two intelligent solutions for this.
1)EDWin defines 7 via pads. You can edit these via pads to suit the requirements of your pads. To do this proceed as follows:
Select the via pad to be edited from the Viapad dropdown in Sizes Toolbar. Now select Tools/ Via padstack. An Edit Via padstack window pops up. Set the hole category, hole diameter, airgap and padstack sizes to suit your requirements and click ACCEPT. Similarly edit other via pads to match the different padstacks you need to use. If you need SMD pads disable the padstack in all the internal layers by setting the pad size in all internal layers to 0. To place these edited via pads, first select the viapad from the Viapad combo box. Select Tools/ Traces .Now select Edit Via/ Create Single via (F1). First, click on the workspace to get a via pad tagged to the cursor. Move the cursor to the required location and click to place it. In this way you can place pads on the PCB. This is one way of solving your problem. But this will allow you to use only 7 pads.
2) If your intention is only to place a cluster of pads you can do this in the following way. Create a new package in Library editor. You can create a rectangular outline and place all the pads of different shapes and sizes you need inside it. Now in Layout Editor, load this package and place it on your PCB.
Q22: Is it possible to adjust via diameter?
EDWin Main -> Layout -> Tools-> Via Padstack (before coming to this option select the required padstack in settings panel ie. #1 to #7 -> Give necessary values for editing -> Accept.
In EDWin XP/2000, Via Padstack can be edited prior to designing the board. This is done by setting using EDWin XP/2000 Task/ Default Via Padstack Editor.
Q23: Is there any troubleshooting utility which will check the project integrity , detect errors and fix it?
EDWin has an Integrity Diagnostics and Autofix tool in Layout à Auto à Net Trace Integrity. The utility will detect and repair all errors like references to non existing nets, empty nets, checks netlist, faulty nodes etc Make sure this is part of your board troubleshooting procedures.