Before using Inventor I used Mechanical Desktop 6 and found the sheet metal functions (AutoSm) to be fairly simple. Since switching over small tasks can now be a nightmare! The main problem I face is exporting flat patterns to dxf format. We use a CNC Turret punch so splined corners on parts are a no-no due to the number of hits required, AutoSM solved this with the 'Apply Smooth' function which created crisp corners suitable for punching. Is there any simlar function available on Inventor? At the minute I either have to apply multiple cut and extrusions to the flat pattern or else 2D modify the dxf file.
Thanks
What version of Inventor are you using?
Can you attach a sample Inventor file here?
The part is not made correctly as a sheet metal part (Extrusion1 is not the correct way to cut this).
So two issues will have to be addressed - modeling the part correctly and getting output of splines as circular arc curves.
I know how to fix the first issue, seems to me they added functionality for the second issue (the original reason for your posting), but I have not investigated that so this will be my first attempt. I hope my memory isn't faulty on the second issue.
Back in a while, maybe someone else will jump in here in the meantime.
Thanks but what is the correct way to create that cut? Also outputting splines as circular arc curves still doesnt fix my problem completely. Ideally the output dxf should have an end profile like the attached (this is essentially the same folding with Apply smooth used on MD6)
It might have been chords (straight lines) that was thinking of.
I think there is a setting to have Inventor turn the spline into chords of a length you specify.
The way you made the cut would not be correct in an CAD program as the cut edges are not perpendicular to the flat face.
I will post an example of how it should have been done.
If you view the flat in wireframe mode there should be only one edge (at indicated locations).
The spline problem occurs where there is a cut across an angled bend (yellow arrow).
Sketch3 - you have extra dimensions. Use Equal Constraints.
I have never used Zeor(o) dimensions since leaving MDT 10 years ago - use Project Geometry and Coincident Constrraints.
Check out this part (of course you would set up with your Excel parameters) and then we can move on to the second part of the problem.
Notice that there are no double lines on that mitered end.
Hi! Here is another solution without having to remodel too much. Basically, you just need to create Thicken features to replace the lump having the non-perpendicular detail faces due to the cuts.
After that, you can right-click on the Flat Pattern node in the browser -> Save Copy As -> select DXF -> OK. You might need to adjust the spline conversion tolerance in the DXF OUT process to get the desirable result.
Please let me know if it works for you.
Thanks!
After looking at Johnson's solution - I realize I missed one feature in my "solution", but you should be able to figure out and adjust.
I have now got the part to where you left off regarding the cuts etc. (attached) Can you advise how i go about outputting the splines as chords?
Hi! Attached is a DXF file output from Inventor Flat Pattern. I used 1mm Linear tolerance (instead of default 0.01mm). Could you take a look and see if it works? If the result is what you are looking for, you can simply do the following to get the same result.
1) Open the Inventor part in Inventor.
2) Activate Flat Pattern to see the Flat Pattern.
3) Right-click on Flat Pattern icon -> Save Copy As -> select DXF or DWG -> Geometry -> change the tolerance from 0.01mm to 1mm ->OK.
Please let me know if it works for you.
Thanks!
Thankyou that is much closer to what I am looking for, I will have a play around but it looks like I have my solution, cheers
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