Is it possible to dimension an external thread automatically in a horizontal or vertical dimension? See below:
I can automatically insert the "incorrect" annotation by: RMB on the thread > Insert Callout
However I would prefer that this information is shown as I have marked "correct" above. To create the above I typed the text in manually, but is there a way to link this to the feature so that if it is changed in the model then the drawing is also updated automatically?
Every Company I know measure the way Chris Burn said DIN/ISO 6410-1.
In our SOLIDWORKS Essential Classes we teach normally how to replace Ø with an M and add the thread pitch to get the Measure they want.
See also: SPR 761155
Chris Burn Please create an SR and add it to this SPR 761155
Hi Michel, thanks for the reply. Can you point me in the right direction for adding an SR?
Also - I dont have permission for to follow the links that you have given.
Functionality is supported directly in SW2020. See page 88 for adding callouts to side views of external threads,and for simplifying the callouts (exclude "machined threads" text): https://files.solidworks.com/Supportfiles/Whats_new/2020/English/whatsnew.pdf
I'll check out the SPR tomorrow to see if there's something more specific that is keeping it open, but otherwise, it should've been closed.
Matthew Lorono wrote:
Functionality is supported directly in SW2020. See page 88 for adding callouts to side views of external threads,and for simplifying the callouts (exclude "machined threads" text): https://files.solidworks.com/Supportfiles/Whats_new/2020/English/whatsnew.pdf
I'll check out the SPR tomorrow to see if there's something more specific that is keeping it open, but otherwise, it should've been closed.
Hi Matthew Lorono, on a more general note, what's the best channel for flagging SPRs that look like they should be able to be closed? While performing searches in the ER list it's not uncommon to find one that, from the information we have available on it, looks like it should be able to be closed out.
Currently, there is no formal mechanism. We normally do close them, but sometimes enhancement request SPRs are missed or we decide not to close. I can go into why, but the reasons are fairly innocuous but highly specific to nuances in software development. I can make some suggestions on how to get in contact with us about this, but I don't want to set up an ad hoc system out of thin air, so let me look into this.
Sounds ideal, thanks!
So, I examined this SPR 761155. It's regarding undercuts or end of threads (where the threads transition to the the untreated portion of the cylinder), not about thread callout itself.
Fair enough then. I've not seen or done it that way, but there's an obvious need. (obviously need to check my standards)
Not an ideal solution, but you could alter the Dimension Text and then save it as a style, (one per pitch). Down side is when you apply it to a new diameter DIM and apply the style the diamter symbol remains, so you need to delete it manually.
I agree with the others that the 'incorrect way' is the correct way. Though you can change the dimension to display most of what you like by editing the dimension text box. The pitch will not update automatically though. I'm not suggesting you do this as standard practice but offering a suggestion in hopes that it may help in another way sometime in the future.
Thanks for the replies.
I shouldn't really have labeled these an incorrect/correct. The standard I am looking at right now says that my "correct" way is correct, but really I just want to go with what is most clear. And I think that in this case (once I have added all the other dimension to the drawing) that dimensioning at the end is the most clear.
Looks like I'll have to continue adding the "M" and thread pitch manually.
The text M10x1.0 Machine Threads comes from the SolidWorks toolbox, sort of. When you add a cosmetic thread or hole wizard feature, it shows you the text that appears. I wasn't able to edit this directly though. I dove into the toolbox and there I could also find no references to Machine Threads or the callouts.
Until the problem is resolved, a possible workaround:
1. dimension external thread and delete the text of the dimension
2. RMB on external thread in drawing > insert callout
3. left in the Property Manager, disable the leader (arrow)
4. Remove the tick from the "Use Document Font" box on the left side Property Manager
5. change the angle of the text
6. align text to the dimension (where the value was removed)
7. select dimension and text
8. RMB > Group
Video attached
Thats best workaround so far
Functionality is supported directly in SW2020. See page 88 for adding callouts to side views of external threads,and for simplifying the callouts (exclude "machined threads" text): https://files.solidworks.com/Supportfiles/Whats_new/2020/English/whatsnew.pdf
It doesn't seem to be working for me, whenever I add a thread callout as instructed by the 'what's new', it shows up in the internal diameter of the thread instead of the outside diameter.
It forces me to add the thread callout in the old way by deleting the diameter symbol and then adding the 'M' and pitch manually.
PS:
I made a few drawings in this incorrect way and had myself a bunch of complaints from co-workers and machining providers alike.
These designation standards cover everything including standard threads, special threads, LH, RH, fits, plated, etc. Properly used, they can't be misinterpreted or misapplied.
ANSI B1.1 Unified Inch Section 6
ANSI B1.13M Metric Section 7
Every US company should have a comprehensive set of ANSI Specifications in their engineering library.
The best method of how to use Solidworks to present this information on a drawing is a completely different set of problems and controversy.
Hi Chris,
by which standard are you defining the 'correct' annotation? The 'incorrect' one looks right to me.