Q1: When I invoke
“Fabrication Manager”, I get the message: "Can't read file
\EDWinXP\SYS\NONE.APT". What’s wrong?
You don’t have to reinstall EDWinXP. Just give path for sys directory in the shortcut
of EDWinXP icon. "Drive: /EDWinXP/EDWinXP.exe" "Drive: /EDWinXP/Sys".
Q2: When selecting define artwork, is it necessary to select
mirror at the solder layer? When should we use the mirror?
If you select mirror, you will be able to view the solder layer as when you look at the
PCB from the solder side. Otherwise, you will be viewing it as when you look at the solder
layer from the component side.
Q3: 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 project, invoke Library editor and remove the component outline from all the
packages
2) Using Layout Editor you can switch off all the COMPNAME text on the board.
3) Add COMPNAME text in component layer using Tools/ Texts 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. )
Q4: Can I generate heat relief pad in fabrication manager or in
layout editor? If yes, how?
You can generate it in Fabrication manager. Heat Relief Pads are used mainly for two
purposes:
To arrest the flow of solder within the internal
layers while wave soldering is done.
To allow heat dissipation.
The procedure is as follows. Select Copper Pour Area tool from Create Copper graphics item
in Tools/ Copper mode. Select the layer and the net (or else last created net will be
taken). Draw the boundaries of the Copper pour and finish. The option of Stretch item tool
allows you to edit Copper Pour Area. Now invoke Fabrication/ Setup/ Gerber Artworks.
Select the layer and click execute to open up another window. Here click EXECUTE to start
processing. Now select Gerber viewer Setup from File menu. The Gerber files are to be
selected in the order given below to get a superimposed view (the result will be always
single artwork file independently of preprocessing mode) or individual files can be
preprocessed.
Gerber ASCII file: COUNTE52.GBR
Gerber ASCII file (superimposed) COUNTE02.GBR
(The above files are generated if the layer selected for artwork is Comp. Layer and if
there is a copper pour area on the board.)
The resulting artwork file has by default always the same name as Gerber ASCII files. In
this case it would be COUNTE52.ART.
In Tools/ Gerber view you may find pads belonging to the same net will have Hrf generated
(provided Hrf is created for the pad in Library editor).
Q5: What do you mean by 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.
Please read ‘Fabrication Tasks’ in Fabrication Manager Help - Optional creation
of Copper Pour Areas.
Note: Use Copper Pour Area and not Copper blocks.
Q6: 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, just
select the files as below:
Gerber ASCII file:
COUNTE52.GBR
Gerber ASCII file (superimposed) ; COUNTE02.GBR
The resulting artwork file has 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 process.
Q7: How can I print out the layout with drill holes in the pads?
(via's and components)
From the Fabrication Manager, select Tools -> Artwork&Pwr/Gnd planes-> Select
layer for diplay. Enable View -> Artwork -> Center holes then go to File ->
Print.
Q8: Pads, when printed are smaller than on the screen?
Load the project, invoke Fabrication Manager and select File/Print. This pops up a window
that displays a sheet outline. 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. Set the above-mentioned print scale. Try this method and check whether you
are getting the pads in the required size.
Q9: How to view mechanical details in Gerber file? I can’t
find the file.
You can create mechanical details in Gerber file using Tools/ Notes, Create Graphic Item/
Create Text. Then, select Fabrication/ Setup/ Gerber Mechanical 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 project
name and the last two being 90 for component side and 91 for solder side. Now view the
generated artwork file in Tools/ Gerber View. Mechanical plot may include board outline,
dimensions, board description notes, holes and pad frames.
Q10: Can we adjust the size of pads in Fabrication Manager? 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 Fabrication Manager. 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. EDWin 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.
Q11: While testing connectivity of the artwork, I get a
"possible unroutes" error. 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 Fabrication Manager 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.
Q12: How is it possible to print realistic pcb's on a laser jet?
The holes dimensions are much bigger than the original size?
View/ Artwork/ Centre Holes menu allows to select three hole sizes viz. 1/1, 1/2, 1/3.
Select these options as per the requirement and select File/ Print.
Q13: How to copper fill over tracks and have a clearance between
the copper fill and the tracks (feature)?
EDWin provides a special tool for copper pouring in different shape. Invoke Fabrication
Manager Tools->Copper menu item and pour copper using the tool "Create copper
graphic item". If you want to pour copper over the tracks you can do it using this
tool. You can change the copper to selected net using the tool "Change net assignment
" after selecting the particular net from the "Net" drop down item in the
toolbar. 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 toolbar) and then route
the trace.
Q14: 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.
Q15: 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, please do the following steps:
Select Fabrication/ Setup/ Gerber Photoplotter Data/ Gerber Artworks. Set the artworks for
the selected layer by clicking on particular layer. Click the Execute button. Now in the
Gerber- Output window which pops up will list the positive as well as the negative plot of
the selected artwork. The Negative layers starts from *50 onwards. Now preprocess the
layer selecting from File-> Gerber Viewer setup and select Tools/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.
Q16: How can I print a block or draw lines on the Comp.Print
layer? I have been trying many things in both Layout as well as Fabrication Manager but
cannot get the lines/ block when I create my Gerber files.
Invoke Fabrication Manager, Tools->Notes and select the tool Create Graphic item. From
here you can draw lines, arcs, blocks etc. This will be effected only for Print layers. To
get this in Gerber view you have to select Fabrication/ Setup/ Gerber Photoplotter Data/
Gerber Mechanical Plot and select the layer and execute it. And view that particular layer
in Gerber view (Tools/ Gerber View). The notes should be placed well within the board.
Q17: What is the hole category? If I use the value 0, it is OK
and perhaps without larger meaning in normal use?
It is possible to group holes into a maximum of 8 categories depending on their type.
Type, here, implies whether the hole is to be plated or not etc.
Q18: Is it possible to print out the D-Code Gerber Aperture
table?
You may open the *.APT file (residing in the Sys directory under EDWin XP/2000 folder) in
notepad and print.
|