CAD help. Designs are not rendering properly in CAM software

Huntsman Knife Co. LLC.

Huntsman Knife Co. LLC.

Moderator
Knifemaker / Craftsman / Service Provider
Joined
Sep 10, 2010
Messages
3,968
Hey guys,

I am new to CAD and drew up several different designs to be cut by a waterjet. I use Autodesk Inventor Fusion. I finished all my drawings and emailed them to the waterjet as DWG files. When they opened them none of the drawings rendered properly. The skeletonizing holes are jagged and many of the curves are rough + the scale is off on some of the drawings. The waterjet is using Mastercam.

I tried opening the CAD files in draftsight to see how they rendered and they suffered from the same conversion issues. I also had one design that I had an Architect friend draw in CAD for me. He used Rhinoceros and that drawing also came out funky when the waterjet guys opened it. The holes were rendered as ovals and some of the curves were off.

Does anyone with CAD and CAM experience know whats going on? It seems like the use of splines could be a big problem. How can I fix the drawings so that they will render properly?

Thanks in advance. I'm not the most tech savvy guy out there and I can't figure out why the drawings don't convert properly.
 
I'm a solidworks user to this advice may or may not apply. Typically when stuff like that happens it's because the program opening your file doesn't recognize all the features. Sometimes exporting your model as a solid body or neutral file, i.e. IGES, can fix the problem. If you haven't already done so, you may want to ask your waterjet cutter what file's he typically opens or ask him what version of mastercam he is using and look up what files are compatible with that version.
 
Im solidworks user also ...and autocad/drafts ight etc..
I second what Irishsteel is saying. You just need to find the appropriate file type to export your drawings as.
 
MasterCAM can usually take about anything but DWG is not a very good format for most folks. DXF is about the same thing and is generally better for most folks to import.

There will be spline vs poly line and segment tolerance settings options buried somewhere.

I can not imagine what would make a circle come in as an oval. Nuke it from orbit.

As a person who has imported a lot of other peoples mess, I can tell you it is very nice when a person can send a clean file.
 
I had this same problem. Tips I learned:
1. Do your best to make your drawing with lines and radius's.... splines rarely got translated properly
2. As Nathan mentioned, find some settings that let you save curves, etc... as polyline... which means it will draw the curve as a bunch of short lines (You can set the number of lines that are used)
3. Export as .dxf
4. Sometimes I had to pay the machinist to clean up the drawing in his software (solid works/master cam) to get exactly what I wanted.
 
As others have said, splines don't play well when exporting to other programs. The best file for a waterjet cutter will be a dumbed down DXF file using arcs, lines & polylines. Make sure the start and end points of features do not overlap & are not duplicated under one-another. Also, you'll end up with the cleanest looking cutout if all of your arc segments are tangent to the adjoining features.

Inventor Fusion has had nearly all of the useful capability removed from the full Inventor package. I suspect that may be a good part of your problem as well when trying to export anything.

Good luck!

You're more than welcome to email the file to me to convert, but I can't do anything until Monday. I use Inventor & AutoCAD Mechanical 2013 almost daily.
 
have you solved this problem? I had to deal with the spline conversion thing today. What I did was just draw many line segments along the spline. Then just delete the spline itself.
 
Onespdfk was kind enough to fix my drawings for me. He's a stand up guy to say the least :thumbup:

I believe he just traced over the drawings with polylines and Arcs and saved it as a better file type.
 
In a nut shell, you got it!

CNC conversion programs can't handle a spline because they don't have simply definable elements (continuous radii, radius points, tangents, etc...). A spline requires a series of complex formulas to reproduce its continuously parabolic form. If you understand how G-code works, it makes sense.

Also, start and end points of arc & line segments can't overlap or have any space between them. The conversion program will get confused & start a new cut when this happens, usually buggering up your part in the process.

I'm more than happy to help any BF member with these things.
 
You must log in or register to reply here.
Back
Top