Author Topic: HOW TO: Create PCB outline from DXF  (Read 4634 times)

0 Members and 1 Guest are viewing this topic.

Online voltsandjolts

  • Supporter
  • ****
  • Posts: 1308
  • Country: gb
HOW TO: Create PCB outline from DXF
« on: March 21, 2017, 01:50:02 pm »
For non-trivial PCB outlines I prefer to use a mechanical CAD package and create a DXF file to import to Circuit Studio.
Unfortunately the CS installer doesn't automatically install the required DXF plugin and CS doesn't tell you that when you try to import, it just behaves as if it worked  :palm:

Quick Guide:

MCAD

1/ Start your preferred MCAD software, I use Solid Edge 2D which is free with registration.

2/ MCAD software typically has Model space and Paper space. I draw in Model space to ensure there is no drawing frame saved in the DXF, just the board outline.

3/ Set the drawing origin to be the lower left corner of the PCB outline, or close to it.

4/ There are no units of length in DXF, just numbers and the units are in your head. For a metric PCB, just draw as if the units were mm.

Circuit Studio

5/ First time around you will need to install the DXF/DWG plugin which is a 3rd party utility called "TeighaX". The installer is located at
C:\Program Files (x86)\Altium\CS\System\Installation\TeighaX_Setup_3.9.0.msi

6/ Open a new PCB document and on the Home tab set the units to be either Metric or Imperial, as required.

7/ File > Import > *.DXF    and select your outline drawing

8/ The Import Dialog might require some experimenting to get the right settings. When it doesn't work, its hard to know whether the DXF or the Import Settings are at fault. So...

I have attached a simple DXF outline (70mm x 50mm) which imports correctly to a metric PCB with these settings:

Blocks:Import as primitives
Drawing Space:Model
Line Width:0.01mm
Scale:mm  (Board outline was drawn in mm. Ignore the red text which never gets the size correct)
Locate:X,Y where you want the DXF origin to be placed
Layers:Right-click on Source Layer Name "0" and select "Not Imported"
For the "Default" layer select the PCB layer as "Outline"


9/ In the PCB editor, select the outline primitives and then on the Home tab select Board Shape > Define from selected objects

10/ You might have a shape imported from DXF which you would like to use as a board cutout. If so, select all the primitives of the shape, then in the search box at the top right of the CS window type "convert" and select the appropriate option.

« Last Edit: March 28, 2017, 02:58:39 pm by voltsandjolts »
 
The following users thanked this post: negativ3, ahbushnell, ubbut, O.B.U.B.


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf