Threads in crossing hole geometry

[office66YRG]

Hi everyone,
Looks like I found a bug. I tested it in a fresh project with just a simple extruded box, and the issue happens every time.

Option I choose in hole menu you can see below. I try to design deep 150 to 300 mm holes with M10X1, 12 mm depth thread. You can know these types of holes from cooling canals used in plastic parts production.  

Everything works fine until I create a hole that intersects with an existing one:

And after I click OK, Fusion starts doing some magic.
I’ve attached a short screen recording showing a few different approaches and the results.

Of course, there is a workaround — I can create the intersecting holes first and then manually add the thread profile by projecting the hole edges into a sketch and cutting/creating the thread section.
But this is not an efficient or natural workflow.

Does anyone have a proper method for this, especially when designing cooling channels in mold components?

[bwalker145]

I can replicate the same behavior:

Oddly, checking both as "Modeled" when applying the hole feature works correctly (at least in the model, haven't checked on a drawing).

This could be your workaround for now, although I agree that the original behavior is a bug that needs to be corrected.

[office66YRG]

I agree that I could use the modeled thread option, but this may cause issues at the drawing stage, because someone could accidentally dimension the thread profile instead of the hole center.

Normally, I never model threads in my projects for downstream processes in our company, such as GD&T drawings or manufacturing.

For now, this is definitely just a workaround.
In my case, I handled it in two steps — first creating 9 mm holes, then adding the thread using a projected sketch.

Thank you for checking this on another machine. Now we can definitely say that this is a Fusion issue.

I hope the development team can take a look at this, as intersecting threaded holes are common in mold cooling designs.

[bwalker145]

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@office66YRG wrote:

I agree that I could use the modeled thread option, but this may cause issues at the drawing stage, because someone could accidentally dimension the thread profile instead of the hole center.

Normally, I never model threads in my projects for downstream processes in our company, such as GD&T drawings or manufacturing.

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Agreed 100%. I avoid modeled threads completely, unless it's a special-purpose custom thread. It can cause dimension/specification issues like you mentioned, as well as make the model unnecessarily heavy.

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@office66YRG wrote:

I hope the development team can take a look at this, as intersecting threaded holes are common in mold cooling designs.

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I'm fortunate that our tool shop handles primary mold design, but I'm sure I would have run into this soon as well working on an EC.

@johnsonshiue  Is this something you could please take a look at?

[TheCADWhisperer]

@office66YRG 

I haven't tried this - but,

Fusion will automatically resize a hole to tap drill size when you add a Thread (cosmetic) feature.

Create the drilled holes with a Counterbore.

Then add the Thread feature and see if it resizes.

Let me know if this workaround actually works.

[johnsonshiue]

Hi! I must not have followed the steps correctly. I cannot seem to reproduce it in Fusion on my machine.

Many thanks!

[bwalker145]

Here's what I'm seeing:

- I tried edge references like your file, and wasn't able to reproduce the issue. I'm using sketch points for hole location.

- ANSI Unified threads did not have the issue, but changing over to ISO Metric profile causes the issue to reappear.

[johnsonshiue]

Hi! The behavior is somewhat unpredictable. If I edit the second hole feature on your model and hit Ok, the cosmetic thread will come up. I am sorry I don't understand the behavior. I will work with the project team to understand it better.

Many thanks!

[gnigmat]

Created a block of 4'' x 4'' x 0.5''. Then, in the middle of the sides (2'' x 0.25'') in XZ and YZ planes, create holes for NPT taper tapped 1/8''. Both holes should have a length of 2.2'' (just as an example). If both are 1/16'' or 1/4'', everything works fine. In case both are of the 1/8'' size next error occurs:
"Compute Failed
Thread size is bigger than the body. Unable to create hole and thread. Reduce hole/thread size and try again."

No issues occur if holes have different diameters.

What could be the issue?

Fusion version: Fusion  2604.1.48 arm64 [Native] 

[gnigmat]

I encountered a similar issue here: https://forums.autodesk.com/t5/fusion-design-validate-document/failed-to-create-two-intersecting-hol.... The problem appears to be due to the specific diameter of the hole (and certain thread types), as the intersection geometry cannot be solved for some reason, resulting in an error. Not sure how to solve the problem...

[office66YRG]

Thank you, @johnsonshiue , for involving your team to help resolve the issue.
And thank you to everyone @bwalker145 , @TheCADWhisperer , @gnigmat  who replied and checked this unusual behavior under different input conditions. 

I believe the Autodesk team will find a solution soon. For now, we’ll have to use workarounds.

[guilherme_sergio]

Thank you sending this our way, and apologies for the late reply. I'm also struggling to reproduce this from scratch on my end.
In any case, thank you for attaching your models, we can reproduce with those. FUS-227780 has been opened and we'll investigate further.

Kind regards,

[guilherme_sergio]

When writing the previous comment something clicked, after trying to reproduce this for quite a while.

I can now reproduce it reliably. The key was to have the inches set as the active unit.

Adding the steps to follow for future reference:

1. Set inches as the active unit
2. Create a box and add two reference points to any perpendicular faces of the box. The points will later be used as reference for the holes, so they should be (roughly) in the same plane for the holes to intersect.
3. Create an ISO M10x1.5 hole with an offset thread using one of the sketch points as reference
4. Create the second ISO M10x1.5 hole with an offset thread using the second point as reference, and extending it so that it intersects with the first one
5. The thread will disappear from the second hole.

Recording of this: 

Thank you very much again!

Kind regards,

[office66YRG]

Thanks, @guilherme_sergio you still working on it. I believe you will be able to find a solution.