|Top Silk Text rotating
|Page 1 of 1|
|Author:||jet31 [ 03 Mar 2017, 06:28 ]|
|Post subject:||Top Silk Text rotating|
We have this problem that the TopSilk text will rotate when we block rotate the whole PCB.
We already arrange the text in its proper place away form pads and holes so that it will not
be a miss-up thing.
but when we rotate the whole PCB the text well also rotate back agains the PCB does covering the pads , holes.
which will make the PCB miss-up.
Is there a way to avoid this thing to happen.
If these problem can be corrected it will be very helpful in our panelizing the PCB.
|Author:||Tomg [ 05 Mar 2017, 17:23 ]|
|Post subject:||Re: Top Silk Text rotating|
I'm guessing that the difficulty you are having is related to DipTrace's inability to allow more than two specific angles for the reference designators; 0 and 90 degrees. Notice when you rotate a single reference designator it will only give you those two choices. If you are interested, here is a possible work-around...
Export the reference designators to Gerber files
1) In the Main Menu of the PCB Layout editor click on View, choose Assembly Layers in the drop-down menu and select only the [X]Component Markings option in the fly-out menu.
2) Click on File, choose Export in the drop-down menu and select Gerber... in the fly-out menu.
3) In the Export Gerber dialog window select/highlight the Top Assy layer, make sure the [X]Use Design Origin option is enabled and click on the [Export] button.
4) In the Save As dialog window enter "TS" for the file name, navigate to the Desktop folder and click on the [Save] button.
5) In the Export Gerber dialog window select/highlight the Bottom Assy layer, make sure the [X]Use Design Origin option is still enabled and click on the [Export] button.
6) In the Save As dialog window enter "BS" for the file name, navigate to the Desktop folder and click on the [Save] button.
7) Close the Export Gerber dialog window.
Turn off the component markings
1) Click on View, choose Component Markings in the drop-down menu, select Main in the fly-out menu and select None.
Import the reference designators as silkscreen drawings
1) Click on File, choose Import in the drop-down menu and select Gerber... in the fly-out menu.
2) In the Open dialog window navigate to the Desktop folder, highlight the two files named "TS.gbr" and "BS.gbr" and click on the [Open] button.
3) In the Source Gerber File dialog window set Import Mode: to Add and make sure all options are disabled.
4) In the Layers box select the Gerber layer named "TS.gbr" and set Convert to: to Top Silk.
5) Now select the Gerber layer named "BS.gbr" and set Convert to: to Bottom Silk.
6) Click on the [Import] button.
Rotate and Move the PCB
1) Select all (Ctrl + A) and group rotate (Ctrl + R).
2) Move the PCB around as a group until you are satisfied with the location, then click in an empty section of the Design Area to deselect everything.
3) Update all copper pours.
|Page 1 of 1||All times are UTC - 5 hours [ DST ]|
|Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group