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.
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
Hi Chris,
by which standard are you defining the 'correct' annotation? The 'incorrect' one looks right to me.