Having a problem with Combine.

[fishtruk]

Hello,

A prospective customer sent me an .stp file. One solid shape. I need to make a mold for this. The ejector pin has to be shaped as part of the finished item. I can't seem to do a boolean subtraction to get this new negative shape. I get an error saying I have to "check inputs with validate tool" and that edges can't be coincident.  I can't find this validate tool thru the help search. I don't know what kind of solid I have and don't know how to find out either...lost in space!

Is there a video of making molds somewhere I haven't looked?  There's one of Taylor Stein making chocolates but I need a video much more in line of the manufacturing process.  Thanks a ton!

Nelson 

[karyeka]

Hi,

I don't think that error message is appropriate. I will find out more about that. We have validate surfaces in Patch workspace in Direct Modeling but that's not what the message is pointing to.

It would help to get your model to analyze the combine failure.

Can you upload the file or share the link or send it to me anand.karyekar@autodesk.com?

I will circle back on mold videos.

Regards,

Anand

[Oceanconcepts]

Are you sure this imported as a solid?  What is the icon for this shape in the browser? 

[karyeka]

I confirm that its an inappropriate error message. It's pointing to some debug tools. Apologies. We fill fix it (FUS-20542).

[fishtruk]

Thanks you guys!    Ocean, it's listed as a "body"    

Is there something I have to do to make it a solid when doing "new design from file"?

[HughesTooling]

If you go to the patch workspace and select stitch then select the part any open areas should have a red edge. If there are unjoined surfaces pick to join. You should see something like this. You might need to make new surfaces if there are gaps. Can you upload the part or some screen shots.

[Oceanconcepts]

Body is just a generic term in Fusion- bodies can be solid, sculpt, or surfaces. See the icon images in my post above.  

Often imported designs come in as surfaces and need to be “stitched” to make a solid, as per Mark’s post. When it comes to using tools it’s critical to know what sort of object you are dealing with. The kind of 3D boolean operations you want to do can only be done with a solid body.

[fishtruk]

Here's a screenshot

[HughesTooling]

Combine does seem quite fussy, if an edge of the tool is on a surface of the Target Body it complains and gives a general modeling error.

This fails because the highlighted surfaces have edges that are on the top surface of the block, if I move the block up or down 0.10mm it works.

[fishtruk]

I didn't see any red lines in Patch/Stitch

[HughesTooling]

No the icon next to the body shows it's a solid. Does moving the pin allow it to work. Can you do a screen shot with the pin in position.

[fishtruk]

Okay, here's the body. I extruded the exact midriff of this shape up to form an ejector in another cad program, saved it and opened in Fusion then tried to subtract to get the inside shape only only to get that error.

I did this because I didn't know an easy way to make a body from the boundary of a solid in Fusion.

I'm trying to get the ejector shape of the inside details of this part.  Do I have to make the ejector a larger size, do the "cut" then trim the resulting shape down?

I'm sure I'm the problem here, thanks for your patience.

[fishtruk]

Here's the screenshot with the pin positioned for the "cut"

[HughesTooling]

If i'm seeing that right you have a lot of collinear surfaces i don't think you'll get that to work. I think your only option is to go to the patch workspace and delete the surfaces you don't need then use what's left to split\trim the ejector pin.

[fishtruk]

Thanks, gotta go home now. Maybe I'll try it at home. Good thing about Fusion...anywhere

[Oceanconcepts]

You appear to have a solid (Body1), so the Patch/ Stitch tools would not apply. 

So to take this further, more information as to the final goal would be helpful- were you trying to boolean subtract this entire shape, or just a portion? Mark's comment about “overbuilding” shapes to be cut to rule out ambiguity is relevant. Maybe we can see what you were attempting when you had the failure? 

[fishtruk]

Howdy!

I'm home now, it's late and I'm still hacking.  I've included a screenshot showing better what's going on. I've put a cylinder in for the target body and trying to cut with the tool. It doesn't work. Errors out.

I've been told my tool body is truly a proper solid. How could I be sure. I've imported it from a customer and I don't know how it was created or saved.... if that's an issue.

Thanks and in the meantime I'll keep on chopping 😉

[Oceanconcepts]

What you are doing there should work. What is the error message you get?  I’m wondering if there is some issue with ambiguity in some of the surfaces as they imported. Can you delete and replace any of the fillets? If you change the appearance to a translucent material, are there any hidden voids or surfaces? That is something I have seen cause problems. 

I would be happy to take a look and see if I can spot anything if it’s OK for you to send or post the file. Boolean tools in Fusion are pretty robust, in my experience, so it’s interesting that this is not working for you. Send me a PM with a link, or I can send you an email link privately.

[HughesTooling · Accepted solution]

The part I used in my examples failed if an edge was on the top surface of the body I was trying to split, it looks like you might have the same problem.

As a quick test move the pin down a small amount and see if it will work then.

Also these areas don't look good, you have a coplaner surface and all the fillet edges that can cause problems.

I think what I'd do is make a copy of the component go to the patch workspace, delete all the faces above the top face of the pin including the coplaner face. You should be able to use whats left to trim the top face of the pin, then stitch into a closed body.

[Oceanconcepts]

I think Mark is correct with his suggestions. It also looks possible (hard to tell from the image) that there is some discontinuity or an extra surface where the vertical side meets the large fillet at the bottom. Sometimes in the solid model space with Fusion it is possible to just select a surface or surfaces you don’t want, press delete, and have the body heal itself- it doesn’t always work, but often enough to try. 

Another approach would be to make a couple of intersection sketches to set the main dimensions and rebuild the part in the model workspace. I often do that with imported electronic components that don’t come in organized in the way I want. I think my approach might be to model the negative space in the part, then boolean it out of the larger rectangular shape. That might also result in a more editable part.