Intersecting threads issue?

[shaische222]

If you make two perpendicular holes of 6mm and 3mm diameter and then try to create M6 and M3 threads, it gives an error that Fusion was unable to create the threads. I believe this is a bug/issue? You can only create one of the threads, but not both. Tried disabling modeling the threads, but same issue.

[Mike.Grau]

Hi @shaische222,

Thank you for pointing to that.

I have tried to reproduce what you described but I could not find any issue.

Could you might share a screen shot with us.

This would be really helpful.

Thanks,

[shaische222]

Tried modeling it with and without the top thread, seems like the perpendicular thread might not be the issue after all. It's something else. I'm able to specify the thread, but if I try to model the thread, it won't let me. See attached screenshot. error: "inconsistent edge-face relationship"

EDIT: I should also mention, the two perpendicular threads do intersect.

[Mike.Grau]

Hi @shaische222,

Thank you for sharing the screenshot.

I was able to reproduce a similar issue.

Could check if the vertical cut´s through the horizontal thread?

This might cause a problem when you want to model the thread.

Another problem could be that the surface and edges at the outer edges might be 

so small. Could you may try to move your thread towards the cylindrical hole?

I hope this helps. Please, keep us updated.

Thanks,

[stockerwellcome]

I'm running into this problem as well. As a simple example, create a 2" square cube. On one face 1/4" from an edge, create a #21 hole.  On the adjacent face 1/4" from the edge, create a #43 hole. Create a 10-24 thread in the #21 hole. Then try to create a 4-40 thread in the #43 hole. It gives an error.

[Mike.Grau]

Hi @stockerwellcome,

Thank you for your response in this thread here.

It sounds and looks like that the thread extrusion lead to an intersection which could not have been computed.

Could you may try to create the thread with a limited length?

Please, feel free to share a Public Link of your file.

I would be happy to test a couple things and share this with our development team. 

Please, keep me updated.

Thank you,

[stockerwellcome]

After a bit more experimenting, I've found that it always works if one does not select the "Model" option when creating the threads. The "Model" option partially works.

If the first thread isn't modeled, the second one can be, but if one models the first thread, the second thread can't be created at all, modeled or not.

[Mike.Grau]

Hi @stockerwellcome,

Thank you for the update, I can see that happening depending on the diameter and thread type

Could you tell we what you mean with "#21"?  Is that hole with 21 mm diameter?

Please, keep me updated.

Thank you,

[stockerwellcome]

After a bit more experimentation, I've found that it works properly if one does not select the "Model" option when creating the threads.  If one does select the "Model" option, it partially works.

If you don't model the first thread that is created, you can create (and model) the second thread.

If you model the first thread, the second thread can't be created at all, modeled or not.

[stockerwellcome]

Sorry. Number drill size 21 is the tap drill size for a 10-32 screw. Number drill size 43 is the tap drill for a 4-40 screw. I'm still working in inches!

The sizes doesn't make any particular difference. The twp holes and threads can be the same size and it fails in the same way.

[adminQYZVC]

I have the same issue, im trying to intersect two modelled threads but just cant seem to produce without making an error. I tried making a new file and intersecting two threads just to make sure its the same error, and it was. The program cant seem to compute two modelled threads, should be a very important bug to be fixed as its actually a very common operation in machining industry, where im working at.

[TheCADWhisperer]

@adminQYZVC 

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

This issue has come up here many times in the past and as I recall the is a simple solution.

Q1. Are you attempting to add Thread features to existing cut cylindrical features?

Q2. Are you attempting to create Modeled Hole features with threads (initially).

Q3. Are you attempting to toggle Cosmetic Hole features with threads to Modeled?

[adminQYZVC]

i have produced a some sort of solution for this issue. i made a 3d solid with a threaded hole, then i made another cylinder threaded solid.

then i intersected both solids, then used the COMBINE command then using the cut operation to come up with a two intersecting threads. although this may seem like a solution im not sure if it actually is, because as far as i remember there is a difference between inside and outside thread,

i hope this heaps though

[adminQYZVC]

i seem to have come up with a solution although i am still completely unsure, i commented my solution below

[Epiales]

This is still an issue. A better solution is to create a positive solid (by using the internal threads to cut from a solid). Once you have all the positive solids in place, they can be combined. After this, they can be combined with the overall solid from which the threads are going to be cut, using cut instead of join.

[TheCADWhisperer]

@Epiales 

Are internal threads and external threads identical?

How will the part be manufactured? (Machined or 3D Printed)

[Epiales]

No. At the very least, there is a clearance set between them, depending on the settings in the XML file for that thread. In this case, it was for 3D printing, but it's mostly irrelevant to the question at hand. Regardless of the medium, there needs to be some bit of clearance between parts, and all the built in thread standards have this. [Just for completeness and anyone reading this who isn't aware... Internal threads refer to the threads inside the piece that the screw or bolt goes in to. Female threads. External threads are on the outside of a piece, the bolt or screw. Male threads.] Since the thread tool of Fusion 360 doesn't allow for crossing of threads currently, I created a positive solid of the internal threads separately, joined them to one solid, and then used this to subtract from the overall solid. I don't have pics of the steps, but here's the final product: