topic Re: partially tapped thru hole with thread feature at exit in Inventor Forum

partially tapped thru hole with thread feature at exit

rhenstenburg — Wed, 27 May 2026 16:53:15 GMT

3 problems when combining a hole feature with a thread feature:

A designer added a thru hole feature that was partially tapped (1/2-13UNC x 1" DP). At the exit, he added a thread feature, also 1" deep. He didn't pay attention and Inventor selected, by default, 7/16x14UNC. OK, the designer was inattentive BUT ...

Problem #1: Why did Inventor not pick 1/2-13UNC by default.

Problem #2: When detailing in a drawing, the hole note would only recognize the thread feature 7/16-14UNC. I tried this on both orthogonal views and on a section and tried several ways to click on the feature.

Problem #3: To experiment, I changed the depth of the thread feature to 1.5" deep (I did not change the tap). The hole note used the tap from the thread feature and the depth from the hole feature. Curious.

I tried this in Inv2022, 2024 and 2026 (example below).

This should be fixed.

Re: partially tapped thru hole with thread feature at exit

SBix26 — Wed, 27 May 2026 21:23:25 GMT

#1: Inventor's thread "prediction" seems to simply choose the nearest thread to the cylindrical face selected, which in the case of a 1/2-13 tap drill is Ø 0.417 in. It would certainly be nice if it could recognize that the selected face is an already existing tap drill and choose accordingly.

#2 & #3: yeah, this is just plain wrong!

Sam B

Inventor Pro 2027.0.1 | Windows 11 Home 25H2

Re: partially tapped thru hole with thread feature at exit

johnsonshiue — Wed, 27 May 2026 21:51:24 GMT

Hi Rob,

The behaviors do not sound right to me. Please share the files with me. I would like to understand it better and work with the project team to see what we can do.

Many thanks!

Re: partially tapped thru hole with thread feature at exit

rhenstenburg — Wed, 27 May 2026 23:07:54 GMT

I did not save my IDW but I attached my test part replicating what the designer did.

Delete the thread feature at the hole exit and recreate it to see if you get 7/16-14UNC as Inventor's suggested thread like I did. Then bring into an IDW and use the hole note to dimension the the tapped features and see if the same thing happens with your installation.

We are still doing production work with INV2024 but I have 2026 on my system (planning the upgrade). I built the attached with 2026. BTW Both of my versions have all the latest updates.

Re: partially tapped thru hole with thread feature at exit

rhenstenburg — Fri, 29 May 2026 21:30:14 GMT

Yes @SBix26 ! For internal threads, the tap drill size is the minor thread diameter. Seems Inventor is using the hole size for the major thread diameter when suggesting. Boo!

Obviously the converse is true for external threads.

Re: partially tapped thru hole with thread feature at exit

rhenstenburg — Tue, 02 Jun 2026 11:36:07 GMT

@johnsonshiue ... anxious to hear back on this issue.

Re: partially tapped thru hole with thread feature at exit

johnsonshiue — Wed, 03 Jun 2026 02:05:09 GMT

Hi Rob,

Many thanks for tagging me! The behavior does look weird. There could be some explanations. Let me quote your posting and reply to each issue.

@rhenstenburg wrote:

3 problems when combining a hole feature with a thread feature:

A designer added a thru hole feature that was partially tapped (1/2-13UNC x 1" DP). At the exit, he added a thread feature, also 1" deep. He didn't pay attention and Inventor selected, by default, 7/16x14UNC. OK, the designer was inattentive BUT ...

Problem #1: Why did Inventor not pick 1/2-13UNC by default.

[JS]: Though the Hole feature is size 0.5, the actual geometry measures 0.417", which is the minimum minor diameter for 1/2-13 UNC, size 0.5 (based on the thread table). It provides enough material to make the threaded hole.

Thread command isn't aware of the existing Hole feature. The Hole geometry measures 0.417", and the thread takes it literally. The default size has to be bigger than the measurement. As a result, the logical choice is 7/16-14 UNC, size 0.4375.

Problem #2: When detailing in a drawing, the hole note would only recognize the thread feature 7/16-14UNC. I tried this on both orthogonal views and on a section and tried several ways to click on the feature.

[JS]: This is probably a bug or a limitation due to double overrides. A thread is applied on a threaded hole, so the last one wins. But I agree the behavior is very confusing. One can also argue, the thread should not be created as such in the first place. The user intent is inconsistent with how the workflow was designed to function.

Problem #3: To experiment, I changed the depth of the thread feature to 1.5" deep (I did not change the tap). The hole note used the tap from the thread feature and the depth from the hole feature. Curious.

[JS]: The behaviors are confusing, since multiple factors are at play. I suspect these behaviors have been like this for a long time.

I tried this in Inv2022, 2024 and 2026 (example below).

This should be fixed.

Thanks again!

Re: partially tapped thru hole with thread feature at exit

rhenstenburg — Wed, 03 Jun 2026 13:03:12 GMT

Thanks for looking into this @johnsonshiue .

For Problem #1, the designer was inattentive and did not correct the tap that INVENTOR chose by default (he did not choose the tap, Inventor did, and he did not CORRECT the tap that was presented ... result: we received an incorrect part that was our fault - both the designer and checker missed the inconsistency).

My reason for posting is that, when applying a thread feature to an existing hole, Inventor should choose, by default, the tap where the MINOR thread diameter is the hole diameter. If you choose a tap for the hole which matches the MAJOR thread diameter, there is no material available to thread (Inventor shows the graphical thread feature but, in reality, an actual tap of the selected size would tap only air).

As I said earlier, the converse is true for external threads (the MAJOR thread diameter should match the existing outer diameter and yield the default thread size presented by Inventor).

For Problem #2, @johnsonshiue implies that the designer is not following the proper workflow. Personally, I would have created a double tapped hole this same way. I would NOT have used two hole features (one from each side). Is the latter what is envisioned as the proper Inventor workflow (using two hole features)?

To make this feature in a shop, they would drill THRU (once) with the tapping hole size THEN tap each end. This matches the hole and thread feature sequence that was applied by the designer (and what I would have done also). Using two hole features is like drilling twice and tapping (obviously a shop would not do this). To me it seems most logical that the hole note attached to a hole feature should have the drill thru information while the hole note attached to a thread feature should have only the tap and the depth of the tap.

Separate issue (FYI): When I download purchased part models which have tapers for NPT (male or female) or worse, with cut threads, I like to (delete the cut threads and) add the Inventor tap feature before checking the part in. I have noted that Inventor never picks the appropriate NPT tap size, even when the tapers are correct. This may be related to the above.

Now I throw down the gauntlet ... I understand that Solidworks has a very robust hole feature where you can combine multiple hole-type features into one. I wish for this every time I have to use multiple, separate hole features to achieve what I require. For example, a spotface with a counterbore and a thread (e.g., bolting something to the spotface with a shoulder bolt where the shoulder is embeded into the counterbore). While this is just an extra step in the solid model, detailing this in a drawing is a little more difficult. I think this is a worthy challenge for the developers. Note: The double tapped hole discussed above is different because it is not all happening from the same side.

Re: partially tapped thru hole with thread feature at exit

johnsonshiue — Wed, 03 Jun 2026 21:40:59 GMT

Hi Rob,

I have to admit the behaviors are indeed confusing here. It seems to me that the Threaded Hole command and the Thread command operate under two different premises. The Threaded Hole command creates the hole geometry, large enough to cut the thread. While Thread command treats the selected cylindrical face as the major diameter and sizes it accordingly.

To explain the differences, I had to resort to our internal AI (see attached Word doc).

Based on the AI's explanation, it seems to indicate that Thread command is more for external threads, not for internal threads (though not blocked). Or it is to add threads to imported geometry (without designated hole sizes).

The Thread logic in Inventor is not as sophisticated as it should be. There is room for improvement for sure. However, I don't think there will be a quick fix here. I will work with the project team to understand the request better and see what we can do.

Many thanks!

Re: partially tapped thru hole with thread feature at exit

rhenstenburg — Thu, 04 Jun 2026 14:25:16 GMT

Again, thanks for looking into this @johnsonshiue . I credit you with an accepted solution (I now know that the thread feature was intended for outside threads) but there are still caveats.

I could see that the thread feature always takes the diameter (ID or OD) as the major thread diameter when presenting its default selection for the tap (OK for OD, incorrect for ID ... but it can be corrected by the user). There is still the issue of the mix up when using a hole note (my Problem #3). Maybe it would be prudent to issue a warning when using the thread feature on an ID but, ideally, having the thread feature recognize whether it is an internal or external thread is the best goal.

A work around solution using two holes not clean either.

Option 1: Use thru hole with partial depth tap first. Then apply a thru hole with partial, but longer tap depth, to the opposite side (same hole size & tap), I get the tap in the solid model but I also get a warning (and a "red cross") because the hole feature portion is not removing material. When detailing, the hole note only recognizes the first tapped hole (e.g., the longer depth of the 2nd tap is never reported). I tried attaching the 2nd hole note to the threads and to the hole, never could get the 2nd tap "THRU" hole designation or the longer tap depth reported.

Option 2:

Drill the 1st hole blind (not thru) with a partial depth tap. Drill the 2nd hole THRU, same location/opposite side, hole size and tap but different tap depth. When detailing with hole notes, only the first hole is reported (NOT thru and and NOT the longer tap length).

I want the hole note to say THRU without having to override (I hate overrides as they often lead to trouble) and I want the proper tap depth reported.

So, even though I am educated better on the Thread feature, there are still issues.