Problem intersection bodies

[simon.doussetCDVPT]

Hy everyone,

I'm trying to use boolean tools for bodies in F360 in order to remove the place of a body on the top of another one.

As shown bellow, the red body is inside the big one and I try to get an intersection or to cut the biggest. My problem is that F360 doesn't want to do it, it says that I have to be sure that both bodies intersect each other. And I'm sure about that.

Would you have solutions please ?

I san't easily redefine that little body because it is extracted from another body that will fit on the big one, and I need clearance between both to be sure to be able to mount it.

Thank you for your help !

Simon

[jhackney1972]

Without the model, there is little chance the Forum users can help you.  Please attach it.

If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[simon.doussetCDVPT]

You're right. You'll find attached to my message the file needed. Don't worry about all mistakes happening after the actual chronological cursor. I first used a way to arrive to what I want but it wasn't a good solution, that is the reason why I'm trying to do it in a better way.

[jeff_strater]

I have not looked at your design (and don't have time tonight), but I have a good idea of what the problem is.  Combine will often fail if the bodies involved have nearly coincident geometry.  These areas appear to have that condition (you can tell by the splotchy appearance).

[simon.doussetCDVPT]

Thank you Jeff for your suggestion. I've tried it and I do have the very same problem.

As you can see on the attached picture, I pulled the upper face to be sure to have à right crossing of bodies. The fact is that when I use the pulling function, F360 doesn't want me to use it on the 3 faces of that little body, I can't understand why. Would you have an idea ?

Thank you !

[simon.doussetCDVPT]

Hi everyone,

I've tried another strategy in order to realize that clearance to be sure that every piece can be mount on my support. I did a massive cobble that i've tried to cut with different faces all around it.

And I still have troubles, F360 tells me that it can't use secant tools. But I did that surface and it's made of continuous splines.

Does someone would have an idea of the problem ?

Thank you in advance,

Best regards,

Simon

[jeff_strater]

If what you are trying to do is to cut a .15mm depression in the top of the body, here is one way to do it, that does not rely on exact matching geometry.  First, create a sketch on the top face, and project the end edges of the Cage_spd_2 body:

Then, use those two lines to split the faces of the main body:

then, use Offset Faces to push down these faces:

resulting in this geometry:

which I think is close to what you are after.  At the very least, it should give you some ideas of how to proceed...

[simon.doussetCDVPT]

Hi Jeff,

Sorry for my late answer.

Thank you for the procedure, I managed to do what I needed to do.

But I still don't understand why my first method doesn't work. Anyone would have an idea ?

Best regards,

Simon

[TrippyLighting]

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@simon.doussetCDVPT wrote:

But I still don't understand why my first method doesn't work. Anyone would have an idea ?

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Yep. It's a near-coincidence problem due to hackish, imprecise modeling techniques!

[TheCADWhisperer]

@simon.doussetCDVPT 

I didn't look at the part in question - but I did notice that you are not doing threads correctly on this part...

[simon.doussetCDVPT]

Hi,

What do you mean by "not doing threads correctly" ?

I think I used the built in function to make threads. Is there another technique that works better ?

Thank you for your advices,

Best regards,

Simon

[TheCADWhisperer]

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@simon.doussetCDVPT wrote:

What do you mean by "not doing threads correctly" ?

I think I used the built in function to make threads. Is there another technique that works better ?

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This is a well-known issue in Fusion going back to the early days.

The root of your thread does not extend past the radius and therefore the mating part will not engage the thread.

Be very careful about how you use the Thread tool (or in the Hole-Tapped).

1. ONLY thread or tap cylindrical features as Cosmetic representation of thread.

2. THEN add fillet or chamfer feature.

3. NOW go back and change the Cosmetic to Modeled for 3D printing (you might also add a bit of offset clearance as 3D printing is not a particularly precise process).

If you are not using 3D printing the only use Cosmetic representation (or for visual images of large threads and then revert back to Cosmetic).

[simon.doussetCDVPT]

Hi @TheCADWhisperer,

Thank you for your precisions. Don't worry, those pieces are machined pieces so the threading tool is used to facilitate the cotation of pieces. I use the automatic modeling of threads only to help during the design process of pieces.

Best regards,

Simon