CAD Forum

march 2022 UPDATE
After upgrading to SW2021 I noticed that dimensioning an EXTERNAL thread using the INNER lines of the thread gives the correct dimension with M, G etc. based on the thread feature standard attached to the EXTERNAL lines.
If you pick a male thread EXTERNAL edges it results in a DIAMETER dimension, so be careful what you select.

--original post---

I have stumped in the SPR 680544 bug apparently:

Dimension of cosmetic thread in drawing is incorrect, shows diameter dimension not thread size (M)

Inactive (as expected)

EDiT:
Is there some workaround to avoid replacing the diameter symbol with M for threads for MALE metric threads?
It seems that solutions only refere to holes...

EDIT2:
it seems that is a sort of intentional behaviour, but according to our drawing standards we do not use annotation for ext thread dimensions.
our engineers are manually replacing the diameter symbol everytime they attach an external thread dimension on the side view of a shaft with G, M or whatever is required by the standard applied.

The alternative I found is to pick the bottom line of the thread and the dimension attached to the inner lines displays the value of external diameter instead...

I can kind of see why this happens, it's basically a hang-up from internal cosmetic thread where of course you will be selecting the correct line to show the thread. Unfortunately in external cases you are picking inside the shaft to show the correct thread.

It wouldn't surprise me if this hangs around for a long time before it gets fixed, that's if it ever does.

This is(for me) currently most annoying thing in SW.
Before this couldnt be added , and then they fixed it wrong
SW does not like ISO

SW does not comply to ISO standards, look at the ISO thread tolerances. Wait, there are no ISO thread tolerances, only ANSI tolerances available in ISO ?????? And the sorting order of the Thread Size ????? We have been asking to comply to ISO standard for over 20 years, but no way. So do not expect it to happen.

Indeed there are a lot of SPRs and self proclaimed solutions on external cosmetic threads.

SPR 1216828: Parts, Feature - Thread: External Threaded Studs - Dimension is dangling as soon as activate option "undercut"

Source: SPRs

SPR 1121279: Drawings - Annotations: The prefix 'M' of Cosmetic Thread annotation inserted by Smart Dimension disappear on the section view of derived part when parent part is closed.

Source: SPRs

SPR 1217827: External cosmetic thread, Diameter not shown right when edges are chamfered

Source: SPRs

SPR 1145096: The dimension of cosmetic thread in the drawing view of the derived (child) part shows a diameter symbol instead of 'M' when inserted (parent) part is not loaded in memory
As a possible workaround, please go to Tools > Options > System Options > External References and set 'Load referenced documents' option to "All". Then, please open and force rebuild (CTRL+Q) a drawing.
Source: SPRs

SPR 1187963: Callout for external thread is shown at the inner silhouette edge not the outer geometry as expected.

Source: SPRs

SPR 1014175: A drawing from a part - The Cosmetic thread shows bigger when the part, in an assembly environment, is controlled by external references

Source: SPRs

SPR 1150593: Smart Dimension of 'Cosmetic Thread' feature does not apply correctly to a shaft

Source: SPRs

SPR 663481: Add ability to directly dimension external cosmetic threads in the same way as a hole wizard hole thread is dimensioned

Source: SPRs

SPR 547294: Cosmetic thread dimensions: ability to create dims in drawing and import dims from model

Source: SPRs

S-077506: In a SOLIDWORKS® drawing dimension, how do I show external thread callout information that specifies the thread type and the pitch?
When creating an external thread callout, the diameter of the thread appears by default. However, the thread designation and pitch do not appear. For a visual reference, see the attached image. To work around this limitation, follow these steps: 1. Assign a
Source: Solutions