Q5: I am trying to figure out how to pour copper into areas that I don't want the router to use.

Create copper areas from the Postprocessing module (Edit Copper Create Graphic item ). Select the option tools accordingly. If no net is to be assigned to the created copper area, select option tool F7 (Create items not connected to any net). Now invoke Arizona autorouter. Select Load copper before loading the database. Now if you start autorouting, those areas where copper was created will be left unused by the router. These blocks placed will not generate any HRF pad(for this purpose a special option is provided "Copper Pour Areas").

Q6: How can I blend (carefully) the component print layer with the component trace layer.(so that I get the names etched out) Is there a way to do this? I'd like to remove the component outlines and leave just the names?

This may be achieved as follows:

1) Load the database, invoke Library Editor and remove the component outline from all the packages
2) Using Layout Editor you can switch off all the COMPNAME text in the board.
3) Add COMPNAME text in component layer using the Edit Text menu in Layout Editor. (Step 1 and 2 may not be carried out if you decide just to discard the print layer. But the board may look displeasing with duplication of COMPNAME text in print and component layers after 3rd step is carried out. )

Q7: What is the difference between view in the positive and negative in the Gerber view?

The Gerber View displayed can either be viewed as a positive or as a negative. Positive plot is the actual plot with the copper areas in black while a negative plot is the airgap plot with the copper areas in white and all the rest in black. To create the photosensitive film, the negative film is placed and then the artwork from positive film file is superimposed on it. If a superimposed view of both the files is required (provided Copper Pour Areas are created), just select the files as below:

Gerber ASCII file: COUNTE52.GBR
Gerber ASCII file (superimposed) COUNTE02.GBR

The resulting artwork file have by default always the same name as Gerber ASCII files. In this case it would be COUNTE52.ART(single file containing both Positive and negative files).

Program checks several things and issues warnings or refuses to postprocess.

Q8: Pads, when printed are smaller than on the screen?

Load the database, invoke Postpro module and select File/Print. This pops up a window that displays a sheet outline in the "Select print scale ". As the scale factor is changed, the system automatically computes the scaled size of the print and displays in the picture size. When this picture size is more than the printer paper size chosen, a page matrix overlapping the drawing outline is displayed. The number of pages to which the drawing is split is indicated by this matrix along with the number of sheet information at the bottom of the matrix. By default the print scale will be 1:1. That is the reason why you are getting the pads in small sizes. If you want to set any other options for printing then select File/ Print scheduler and double click the option row for layout from the table. From this window also you can set the above-mentioned print scale. Try this method and check whether you are getting the pads in the required size.

Q9: I have a problem while creating power and ground planes?

This just implies that if you assign layer say Comp. Layer to Ground (SPL0), then by default the entire layer will be SPL0. Only pads, which are connected by traces, will have airgaps generated for it. All pads belonging to SPL0 which do not have traces coming to it will be connected to SPL0 by Hrf (Heat Relief) pads. Airgaps will be generated only for those pads that don't belong to SPL0.

Note: Use Copper Pour Area and not Copper Planes.

Q10:. How to view mechanical details in Gerber file? I cant the file.

You can create a mechanical details in postprocessing using Edit/ Notes, Create Graphic Item Create Edit Text Block (option F5). In Gerber View, select Gerber Define Mech.Plot enable the check box Board Description and click EXECUTE. By default the created Gerber file has .GBR extension with the first six letters of the file name being the first six letters of the database name and the last two being 90 for component side and 91 for solder side. Now view the generated artwork file in Edit Gerber View. Mechanical plot may include board outline, dimensions, board description notes, holes and pad frames.

Q11: Can we adjust the size of pads in the Postprocessing? If yes, how? When we sent the Gerber data to photoplotter, can the size of pads modified be recognized by the photoplotter? If yes, how does this happen?

You cannot make any adjustments to pad sizes in the Postprocessing module. Editing operations has to be done in the layout.

The de facto standard for photoplotter data is Gerber format. While generating Gerber files, these pads will be converted to Gerber format. These Gerber files are generated using the aperture sizes available in the Aperture Table. These apertures are defined in terms of a format recognized by the photoplotter called DCodes. All the available Dcodes and the sizes they represent are listed in Aperture Table. The interpretation and repertoire of Dcodes may vary depending on the make and model of the photoplotter. For example Dcode D100* may result in one machine as a .062" line and on another as a .100" line. There are photoplotters that allow flexible Dcode to aperture assignment. For certain others the repertoire of Dcodes may be fixed. Latest photoplotters available in the market may recognize various Dcodes for creating different shapes. EDWin32 defines three DCodes for each available aperture size, namely for plotting lines, flashing round pads and flashing square pads that are recognized by almost all-standard photoplotters.

Q12: While testing connectivity of the artwork, I get a "possible unroutes" error. Under postpro, after I poured the SPL0 copper, I get two wires as "possible" unroutes. Is this a via problem? Or an airgap problem?

This warning shows those nodes of the selected reference net that are not connected to the poured copper. Connectivity Check in Postprocessing verifies that the pads included in the selected reference net are properly connected to the poured copper and checks whether any of the other nets are shorted to the poured copper. Suppose you have defined SPL0 in the component layer and are also referring this net for copper pouring. Then the list of possible unconnects just warns you that certain nodes in the net are not connected to the copper. It doesn't mean that these nodes are logically unconnected. If a part of the net is routed in the solder layer and you select any node of this net, then again, this warning get displayed with the nodes on the solder layer highlighted.
Note: Remember that this artwork check considers copper pouring for the selected layer only.

Q13: How is it possible to print realistic pcb's on a laserjet? The holes dimensions are much bigger than the original size?

Please take print outs from Print Scheduler in which you can have three hole sizes (Original size). EDWin32 Main -> Postpro -> File -> Print Scheduler, select what to print and enable Holes check box, you can have three sizes viz. 1/1, 1/2, 1/3.

Q14: How do I do copper fill over tracks and have a clearance between the copper fill and the tracks (feature)?

EDWin32 provides a special tool for copper pouring in different shape. Invoke Postpro module Edit->Copper menu item and pour copper using the graphic tools "Create graphic item" provided in the left hand side. If you want to pour copper over the tracks you can do it using these tools. You can change the copper to selected net using the tool "change item net assignment" after selecting the particular net from the "Select Net" drop down item from the parameter window. The clearance between the trace and the copper will be the airgap. You can change the airgap of the trace before routing. Change the Airgap (from parameter window) and then route the trace.

Q15: Is there a possibility to generate automatically a ground plane? If no, can I generate it by growing the width of the track?

The system will not generate ground or any planes automatically. You can make this by growing the track size. But it is suggested to use copper pour or use one plane itself for connecting grounds.

Q16: What is the procedure to get a negative layer in files with the center hole in it and to print to my laser printer too. ?

If you want a negative plot for a layer then you need to have a copper pour area on the board and assign it to any of the existing nets. Please do the following steps:

Select Gerber->Define artworks , it will pops you a window where you can set the artworks for the selected layer by double clicking on particular layer. For e.g. double click on Comp. layer and this will get added to the row. Now in the Gerber- Output window which pops up will list the positive as well as the negative plot of the selected artwork (note that "mixed mode polarity" option is not checked in the gerber setup window). The Negative layers starts from *50 onwards. Now preprocess the layer selecting from File-> Gerber Viewer setup and select Edit/Gerber view to view the negative layer.

Switch ON View->Artwork->Centreholes. Now you will get the negative layer with its center holes.

To print, select File->Print Scheduler after setting the various available options of the diagram (such as layout, template, Gerber view, artwork).

Q17: After performing "Check connectivity Test on Artwork" in Artwork Pwr/Gnd mode I find that there are 100's of shortcuts to copper plane. I am not sure weather it is a problem of Edwin or it exist a real Copper contact Problem.

When you execute the Artwork Connectivity Test, EDWin creates a bitmap with a precision of 8mil to 1 pixel. When analysed, the package C_FQFP_100_1 has a pad to pad distance of about 6 mil which is less than 8 mil. In such circumstances while preparing Artwork for Connectivity Test (creating bitmap), all pads get shorted in the bitmap. You can view this after Artwork has prepared for Connectivity Test.Hence the system reports this as errors. This is a limitation of EDWin.