DesignSpark Electrical Logolinkedin
Menu Search
Ask a Question

17 Sep 2018, 13:19

How the DSPCB Community can help you

Sometimes we all need a helping hand when using a design software (we can’t all remember everything!), below is such an example where one of the users of DesignSpark PCB couldn’t figure out how to import a DXF outline so he asked the community. And, the community answered.

Importing a DXF Board Outline

Jordan

I am trying to create a board outline from a DXF, and I am having no luck at all.  I am not given the option to import it as Type Board.  It only detects DXF layer 0.

I am able to select import as a board, but then it gives me the following error:

Warning (line 10006): Board Outlines must be closed and non-intersecting. Some shapes of these types have been created. These have been removed and replaced by open shapes on a non-electrical layer.

Nothing shows up at all.

I am able to select import as a shape on the top silkscreen, but when I do nothing shows up.  Incidentally, there is no error.

Has anyone been able to create a board outline from a DXF, and if so, can you give me some insight as to how?

 

Boss

Is the board continuous, it sounds like it is not a complete shape. You could check your DXF with a dxf viewer, there are some online viewers.

Also, try importing your dxf on to the silkscreen and you should be able to view any shape and look for any issues.

I have only done this a couple of times and it did work correctly. There is an FAQ https://designspark.zendesk.com/hc/en-us/articles/115003735569-How-can-I-Import-a-board-outline-using-DXF- which shows the steps that also worked for me.

From your description, it does sound like the dxf is the issue and worth checking.

Jordan

I am not able to get it to show up on the silkscreen layer.  No errors, but nothing shows up.

In Drawings, the DXF appears continuous.  It really should be, as it is created from an SLDDWG drawing that was created from an SLDPRT part in Solidworks.  It is a picture of 3D geometry, so I can't imagine how it could possibly not be continuous.

I was able to create a custom mapping file that has the Type _BOARD in it, but Designspark is saying that it is an illegal mapping file.

I'm actually looking at the page you suggested, and I'm in the middle of installing Design Spark Mechanical.  I'm hoping I can import the DXF there, the re-export.

 

Brad Levy

The most common cause of not seeing anything show up after DXF import is an incorrect scale factor.  If a length of one in the DXF file represents one inch, but the PCB design is in mils, a two inch square PCB outline (in the DXF) will come across as a 2 mil by 2 mil outline in DS PCB, which is easy to mistake for nothing at all, especially if it ends up down in the lower left corner of the drawing space but you are viewing the centre of the space. Try changing the number in the Scale box of the import dialogue from 1 to 100 or 1000.

The warning about the board outline needing to be a closed and non-self-intersecting means what it says. An outline may have a gap between the starting and ending points smaller than the on-screen line width in your CAD program, in which case it will look closed but not be closed. 
Self-overlapping could be caused by drawing a notch in the board outline as a box, overlapping the main board outline, instead of modifying the main board outline to jog in, over, and back out where you want the notch.

Bringing it in on the silkscreen layer is a good debugging approach. Once you get the outline from the DXF showing up on the silkscreen layer, you can edit it there to correct issues like an almost but not quite closed outline. Then you can change the shape type to Board.

I've definitely gotten importing a board outline from DXF to work as advertised.

 

Brad Levy

A screenshot of the DXF viewed in a viewer might help us see what might be the problem.

 

Jordan

Nice one.  It was a mils vs inches issue.  I didn't bother with a map file and set the scale to 1000. Bingo-bango there's my board outline!

Thank you guys so much for your input!

 

Boss

Glad you got there! It is a good method, but let down by the DXF not having any defined units or precision.

If you rename the dxf to .txt you will see the actual file content with some very high precision numbers! Ignoring that, once units and scale are sorted it's a very useful process. It can also be used to get a logo on to the silkscreen.

One other 'gotcha' is the line width is typically zero which DSPCB interprets as some minimum value so the import still gets displayed, but, it's good practice to change this in the Design Technology to a meaningful value.

See the discussion on the DesignSpark PCB community forum

 

If you have a design conundrum that you just can’t figure out, why not ask the community?

Visit the DesignSpark Community Forum

Downloads

Countless years taking things to bits to see how they tick...now Fighting the good SEO & content battle at Kempston Controls!

17 Sep 2018, 13:19