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 

[fishtruk]

Mark and Ron,

Thanks, I nudged the cylinder down and it worked.

So you can't have any lines coplanar with the target or tool?  Is this a glitch?  I've never come across this in my other cad packages. (not that they're perfect...that's why I am trying F360)

Thanks,

Nelson

[HughesTooling]

I think part of the problem is because it's an imported part, I tried to make something similar in Fusion to demonstrate the problem but I couldn't get it to fail. I have come across this a few times with other software usually with imported models as well.

Mark.

[fishtruk]

Thanks Mark,

I asked the customer's designer to send an alternate format than .stp. but haven't gotten it yet.

I'm having a slow learning curve drawing solids in 360 though. I'll have to shed more.  Know of any double secret training videos on this?  🙂

Nelson

[HughesTooling]

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@fishtruk wrote:

I'm having a slow learning curve drawing solids in 360 though. I'll have to shed more.  Know of any double secret training videos on this?  🙂

Nelson

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What sort of experience do you have with cad before Fusion. Personally I had quite a bit of experience using solid modelers before Fusion, the main difference\chalange is managing the time line across an assembly. One piece of advice is to use components to make managing the time line easier, here's a link to a helpful Screencast

Mark.

[Oceanconcepts · Accepted solution]

Yes, keeping things as components and understanding to activate them when working on that part of the design will make staying organized a lot easier. 

There are many strategies for working with Solids in Fusion. If I were trying to duplicate your part accurately but built in Fusion I might try: 

1) Set up construction planes that intersected the imported model at critical points- wherever I needed a new profile to be able to duplicate the shape. I think this could be done with 3 or 4 planes. If the part is symmetrical I might create a center plane and only build half the part, then mirror it. 

2) Make a Sketch on each one of those planes, and select the Intersect tool to get a sketch cross section. The select those lines and break the link. I would probably delete fillets from the sketch and use the extend tool on the straight lines to create a closed profile. Generally I find fillets work better when made on the solid itself. 

3) Extrude these profiles, using the “pull and click on the surface you want to match” aspect of the extrude tool to match the solid thickness to the imported part. That click-match only works with co-planar surfaces, so if sides are drafted you would need to extruded beyond and use the drafted surface as a trim tool. If there are other drafts that need to be added, that weren’t picked up in the sketches because of orientation, then I would extend the extrude and use the imported surface as a trim tool to split the body. 

That should get to the blocked out shape of the part, then it’s a matter of combining to make a single component, then adding fillets using the push-pull tool. 

I might find it easier to build the negative space inside the part as a solid, then subtract it from the larger block. It just depends on the shape. 

This is a general approach I have used for imported components to rebuild them so they are native and free from import artifacts, yet accurate to the imported part. Others probably have much easier/ faster/ better ways that make this approach look silly. Using zero offset surfaces would be another path, for instance. But in general the tools that let you joint, cut, and intersect can be used to sculpt shapes quite reliably. The fun of this (it is fun, right?) is in discovering how to combine the capabilities of the tools to solve particular problems.

[fishtruk]

My CAD experience goes back to AutoCAD 12 at Penn State. I used it primarily for creating prints and parsing complex parts in 2-d, filling in the gaps in my head when creating the parts in 3-d.  My solids experience is mostly in BobCAD since it was cheap enough for my company to afford. The drawing utility sucked or wasn't something which fits into my head (tryin to be humble and nonjudgemental) but I did model a few dies with very small details and created Gcode to cut them. Mostly I would draw in AutoCAD 12 or another similar, then export a .dxf for use in BobCAD. I've ceased to use BobCAD and won't go into the reasons why here.

Anyway I got clued in to 360 from CNCZone and we could afford it so I went for it thinking it wasn't too far from AutoCAD 12.  Well it is but I have to learn this.

I hope the CAM side is getting better. In some videos I see the selection of surfaces is critical the way 360 parses it. I have however done a few simple tool components with it. No mold cavities yet.

[fishtruk]

Thanks Ron. I will definitely take your comments to heart.

[gautham_kattethota]

Hi,

In terms of best practises, I just wanted to put out a note that, when working with Combine, or for that matter any kind of boolean (Join/Cut/Intersect) operation, it is always better to have some kind of an overlap between the bodies you are trying to boolean.  The boolean engine could encounter issues with 'touching' cases, where one or more faces of the two bodies are coincident (or on top of each other).  Many such cases might work, but there are possibilities that some might not.

Regards

Gautham

[gautham_kattethota]

Another point is that with imported parts, there are possibilities that there might be issues within the model compared to a body natively built in Fusion.  The model itself might check clean but there might be geometric tolerance issues within the model.  When you have bodies that have some coincident faces when trying a boolean and when one or both the bodies are imported, there are just more chances that a combine might not work.

Regards

Gautham

[fishtruk]

Okay, more data for the dead horse.

I got several flavors of files from the customer. everything does not work Except...Importing an .stl file in Bobcad, then saving it as a .stp file.

Then the Booleans work!  I've got a postit on my wall now for this.

Thanks.

Nelson

[kb9ydn]

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@fishtruk wrote:

Okay, more data for the dead horse.

I got several flavors of files from the customer. everything does not work Except...Importing an .stl file in Bobcad, then saving it as a .stp file.

Then the Booleans work!  I've got a postit on my wall now for this.

Thanks.

Nelson

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Importing an .stl in Bobcad... so two wrongs really do make a right? 

Sorry, I couldn't resist.  My guess is that there is some less than optimal modelling going on with the original file.  It takes a lot of skill and experience to make complex shapes that are also geometrically clean.  And even very mature CAD programs can make crappy models (as me how I know).

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