Posts from — June 2010
Extruding the PCB – Overview
The first step to a complete 3D PCB model is to create the PCB.Â The basic approach is to export a DXF outline of the PCB and its holes from Eagle PCB, import it into Alibre, and then extrude it.Â It’s not as easy as it sounds.
Alibre Design refuses to extrude sketches with any overlap.Â AD V11 did not show where the errors are, but V12 does (this feature alone makes V12 worth the upgrade).
If your PCB border has a non-zero width, Alibre will not extrude the PCB because the four corners overlap.Â For some reason, Alibre Design does not accept the way the standard Eagle DXF script creates holes.
I did not have any success getting Alibre Design to extrude the silkscreen or trace layers, nor was I able to overlay the silkscreen or traces as a visible sketch on top the extruded PCB (maybe because Alibre Design does not support surfacing).
When extruding, CoCreate PE is about as picky as Alibre, but (like AD V12) it highlights what it doesn’t like.Â SolidWorks doesn’t have problems extruding the standard Eagle DXF output.Â VX Innovator is also less picky; I have successfully extruded the silkscreen layer.
I made a couple quick and dirty changes to the standard Eagle DXF creation ULP to fix the holes; the result is dxf-fsw.ulp.
Creating the PCB — Step By Step
- Open your project in Eagle, then open the Eagle Board editor with your PCB layout.Â I used the FP-SMC-1 project as an example; you can download the files here.
- Make sure your borders have a width of 0.
- In the Eagle PCB board editor, turn on onlyÂ the dimension, via, and pad layers (layers 17, 18, and 20).
- In the Eagle PCB Board editor, run the dxf-fsw.ulp ULP.
- Select a file name for Output file; I used FP-SMC-1.dxf with the appropriate path for my Eagle PCB setup.
- The Always vector font, Use wire widths, and Fill areas setting should not matter.
- The units do matter: you need to know them when you import the DXF.Â I used inches.
- Then run the script by pressing OK.
- You can download my resulting file here FP-SMC-1.dxf
- Close Eagle PCB.
- Start Alibre Design.
- Select the File->Import menu, select AutoCAD DXF files for the file type, select the file (in my case, FP-SMC-1.dxf), and press Open.
- File Units need to match the units you used when creating the DXF in Eagle (I used inches).
- I don’t think Maintain Projection matters.
- Importing Only Visible Layers makes sense.
- Start importing by pressing OK.
- Select the Sketch->Activate 2D Sketch menuÂ (or press Ctrl+K).
- Select the Edit->Select All menu (or press Ctrl+A)
- Select the Edit->Copy menu (or press Ctrl+C)
- In the Alibre Home window select the File->New->Part (or press Ctrl+Shift+T)
- Select the Sketch->Activate Sketch menu (or press Ctrl+K)
- Select the plane to use for your new sketch.
- You can name the sketch.Â It’s not a big deal in a simple part, but I would recommend named sketches in a complex part.
- I used the XY plane.Â You can select the plane by either clicking on the plan in the work area, or clicking on the list of planes in the tree on the left (e.g. Planes->XY Plane).
- Select the Edit->Paste menu (or press Ctrl+V) to paste the DXF drawing into the sketch.
- You could select and move the sketch around if desired.
- Select the Sketch->Activate Sketch menu (or press Ctrl+K) to deactivate the sketch mode.
- Select Extrude Boss by menu (Feature->Boss->Extrude) or icon (typically the top right icon).
- Verify the correct sketch is selected.
- Use To Depth for Type.
- Use your PCB thickness for depth (0.062″ or 1/16″ for me).
- I reversed the extrude so the sketch is on top (probably doesn’t matter a lot).
- Leave everything else with the default settings, except you may want to name the extrusion.
- Start the extrusion by pressing OK.
- Save the PCB using the File->Save As menu (Ctrl+Shift+S); mine is available as FP-SMC-1 PCB.AD_PRT
- We are done creating the PCB itself.Â Now we have to assemble the board inside of Alibre, so stay tuned.
Here is the FP-SMC-1 PCB as an Acrobat 3D PDF; if a correct version of Acrobat is installed, you can click on the PCB, and then rotate it and more.
June 29, 2010 3 Comments
I’ve added the Eagle PCB source files for six PCB projects, included the five boards I’ve discussed previously.
I plan on experimenting a bit with the format of the download page.
And, yes, I am still working on the Eagle PCB/Alibre series; in fact, I created the download page to support my next post in that series.
June 19, 2010 2 Comments
What Is This New Series About?
I will create a 3D PCB model using Alibre Design Standard V12 from an Eagle PCB project (I will be using the FP-SMC-1 an an example).Â I will not cover every single little step in detail, but I plan on being complete and fairly detailed.
The same basic approach will also work with other MCAD programs; along the way I will include some notes about other design software.
Why Create A 3D Model?
After all, the PCB fab houses want Gerbers, not STEP files.
A mechanical model canÂ be used many ways, including:
- Checking your PCB footprints (especially if you use STEP or IGES models from the manufacturer)
- Check the mechanical layout of the PCB and the fit of the PCB into a larger mechanical system.
- As an input to simulation software, including thermal modeling.
- To create a beautiful, accurate rendering of your PCB.
- I will not be covering this.Â In fact, Alibre Design Standard does not include photo-realistic renderings; you have to have Design Professional or Expert.
Why Not Create a 3D Model?
Creating a model can take a lot of time, although once you’re experienced and have models for all your common parts, the time should be reasonable.
If you want to be able to share your results widely (e.g. export to STEP files), it will cost some money for the necessary MCAD software.
Spending more money can save a lot of time; for example, if you create your parts correctly, you can use the Eagle 3D ULP to create IDF files representing your board and its components.Â Then using even more expensive MCAD software (such as SolidWorks + CircuitWorks), the MCAD software will use the information in the IDF files to automatically create a board model.
Since life isn’t perfect, the board might need some tweaking.Â Also, I’ve read that Eagle’s IDF output sometimes needs some tweaking before the MCAD program likes it.
There are at least two programs for creating PCBs in Alibre using IDF files:
If you are creating a lot of PCBs at work, I would highly recommend looking at these programs.
What If I Just Want A Pretty Picture?
There are at least two free options for photo-realistic renderings with Eagle PCB:
- The original Eagle 3D project which uses POV-Ray.
- The new Eagle’up project which uses Google Sketchup.
There are some disadvantages to these programs:
- They are not useful for mechanical engineering (using the board as part of a larger MCAD model)
- They do not have large part libraries, and the companies that do provide 3D models typically use STEP, IGES, or Acrobat 3D.
- However, some file translation could help.Â For example, if you can convert a STEP file into STL (which CoCreate PE can do for free IIRC), you can try using the STL to POV conversion utility for Eagle 3D.Â You should be able to do something similar with Sketchup.
Why Alibre Design and Eagle PCB?
The short answer: because I have them and like them.Â Both programs are reasonably affordable, and fairly popular.Â I’d be happy to write about all the other options if I was well paid to do it!
What Are Some Alibre/Eagle Limitations?
So far I have found a few:
- Alibre Design Standard does not do photo-realistic renderings
- I have not been able to get Alibre Design to handle PCB traces so far; I can’t extrude them (as produced by the current DXF exporter) and I can’t overlay them.
- This could make it harder to model SMT PCBs; on through hole PCBs, it’s obvious where the parts go.
- Alibre Design Personal Edition (PE) is not usable, since it cannot import STEP files; the cheapest options are either Alibre Design Professional (about $500) or trying to see if you can still grab a copy of Alibre Design Standard (e.g. Novedge still lists it for $185)
Are There Other Affordable Options?
If you want to create a solid model that you can export in STEP format, only other MCAD choice I know of that’s under $1000 and might work well is VariCAD.Â The other choices have various limitations, which I might discuss in another blog post.
Or you could use different PCB design software; some programs will do at least some 3D modeling.Â For example, there is Altium at the higher end (about $4,000) and Target 3001 at the lower end.Â KiCAD (open source) has some sort of 3D capability.
Target 3001 does look interesting, since prices range from free to about 3,000 euros, and it can export to STEP files.Â Sometime in the not too distant future I hope to take a look at it.
June 5, 2010 6 Comments
Three years of blogging — and I’m still averaging about a post every week and a half.
I’ve been very busy in the first half of 2010 with family and work, so I haven’t been able to post as much as I would like.
I am working towards finishing a few posts on creating a PCB model in Alibre from Eagle PCB, but as normal it is taking longer than I hoped.
Once the Alibre/Eagle series is complete, I will be doing a practical motion control series.
June 1, 2010 2 Comments