Making and patterning a zero-width cut (for waterjet/laser cutting)

[DRoam]

We make a piece that has a bunch of sideways "H"-shaped cuts in it, like pictured below.

However, we make these cuts with a waterjet, which means we essentially want them to be zero-width (lines), because otherwise the waterjet will trace BOTH sides of the cut, which isn't necessary and doubles the production time.

But I haven't been able to find a way to do this in Inventor. I can't even make that shape of cut using the Split tool, and even if I could, we can't pattern a Split in Inventor.

I tried using the Sheet Metal environment to make a rectangular cut and then create the two flaps as straight Flanges, and I could almost get this to work, but I couldn't get the top/bottom gap to be zero, and the two flanges would always fuse together in the middle.

We need this part in our Inventor assembly for visual purposes, plus it's parametrically connected to other parts of the design; so modeling it in Inventor is not optional. But we'd really like to avoid having to re-draw it all over again in AutoCAD just for the waterjet drawing. Not only is this a pain, it also results in wasted time, potential for mistakes, and/or project delays.

We'd like a solution where we can either:

A) Model the part with zero-width cuts in Inventor (preferred), or

B) Export the Inventor model with finite-width-cuts like we have to make now, and somehow auto-magically convert them to zero-width cuts (lines) in AutoCAD

Any suggestions are appreciated.

[jmfowler1996]

Try this:

1. Make an 'H' shaped sketch on the part, with only three lines.

2. Extrude each line of the sketch as a surface.

3. Use the "Split" tool to split the face on the part by each surface.

You should end up with a zero-width cut. I think inventor also treats the splits as only one line each.

You might not be able to pattern the splits, but you can pattern the surfaces and split the face using each of the patterned surfaces.

Good luck!

[JDMather]

I think it might be easier in the drawing environment. (particularly given that the design intent is for a pattern)

[jmfowler1996]

Maybe, but if the part is connected parametrically to other parts, he might want the split in the model itself?

[JDMather]

I have another idea of modeling the geometry as it is in the real world for the purposes of the assembly.

Also model surface bodies for the single line waterjet process.

Hide the slot boundaries in the drawing (should be able to window select).

In the drawing include the surface (this will give single lines in the slots).

Save the dxf.

I didn't try this, so might require a bit of toggling layer visibility - but it should work.

I still think a pattern in drawing would be easier than creating the surface bodies though and the slot edges could still be hidden in the drawing before export to dxf.

[DRoam]

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@Anonymous wrote:

Also model surface bodies for the single line waterjet process.

Hide the slot boundaries in the drawing (should be able to window select).

In the drawing include the surface (this will give single lines in the slots).

Save the dxf.

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That's a great suggestion, JD. I'll play around with that and see if I can make it work.

I think the hard part will be making it so if I increase the number of H's in the pattern, it will automatically hide the slot edges and show the cut surface for the new instances. I'm not sure that will be possible. But even if I have to manually do that -- if manually doing it is faster than re-drawing/fixing in AutoCAD, that will be an improvement.

I suppose I could try the in-drawing Sketch pattern... but I don't think I could make that parametrically driven which is important for us.

Thanks for the suggestions.

[asiu · Accepted solution]

@DRoam

I found another way of doing it.

You draw the "H" profile in a part sketch and you pattern it in the same sketch:

If you can do your CNC code from this file fine, else you can "Save Copy As" a AutoCAD Dwg file.

Upon opening this in AutoCAD you get this:

What you get are lines you can surely program, as you were doing you CNC programs out of AutoCAD.

Hope it helps.

Regards,

Adrian

[DRoam]

@asiu, that's a great suggestion, I don't know why I didn't think of that. I think that will work perfectly. Here's how I implemented it:

1. Model my part up to everything except the H's (including any bolt holes, other cuts, etc.).
2. Create a waterjet Sketch on the top face and do a "Project Cut Edges". This ensures that ALL of the geometry is in the waterjet drawing, including the outside border, bolt holes, etc.
3. Create the single-line H sketch and dimension and pattern it using the driving Parameters.
4. Now create another Sketch with the full H-cut profile (with a finite cut width about equal to our waterjet cut width), extrude-cut it, and pattern that extrude feature using the driving Parameters.
5. In my Waterjet .IDW drawing, create a view of the Part, right-click the Part in the Browser, and select "Get Model Sketches". Hide all the sketches except the Waterjet sketch.
6. Now edit my Object Defaults and Layers such that Visible Model Edges are not displayed. Now only the waterjet Sketch will be displayed. I also had to right-click and say "Display Reference" so the projected geometry would be displayed.

Now the vent's sizes and pattern will always be up to date and correct in both the Part itself and in the waterjet drawing. And the Part itself will have the true-to-life cut width from the Waterjet cut, while the Waterjet drawing will have the necessary single-line cut path for tracing.

I think this will work well for our purposes. Thanks JD, asiu, and jmfowler for your suggestions.

[asiu]

@DRoam

Happy that was useful.

I learn something too, as we do parts that are water-jet cut. So thank you!