Adding thread information to a drawing.

[tomstickland]

I've spent some time looking into this.

I have a part in a specification file and I'm doing drafting.
The requirement is to link thread information to the model.

Here's the method I used. It's rather involving:

Look in the model, find the expression name for the thread. Eg: p106 = "M6 x 1".
Also expression name for thread length. Eg: p300= 9
Edit the names to something more descriptive if required.

In the drafting view add a hole note (or radial or diameter dim). Or add some text, but the leader then doesn't auto point to the centre of the thread.

Edit the style to have user defined radial symbol and set it blank. This is to get rid of the R or diam symbol.

Use the annotation text editor to overwrite the dimension text.

Edit the text, use the text editor. Click on the "relationships" tab.

Click on "expression".

Click on "link to part". Select the master part.

This gives a list of expressions, but often the thread parameters are missing.

Pick a random expression (because the wanted expression is not available in the list)

Edit the script so that the correct expression is referenced.

OK it all.


If there's a better way of doing it then tell me. I did try "Insert Feature Parameters" but that won't bring in a nice "M6 X 1", it'll add two diameter dimensions, one of "M6.1" and one of "dia 5.2".

 

[jerry1423]

Check the last reply to this posting.
I was somewhat frustrated too.

http://www.eng-tips.com/viewthread.cfm?qid=265882&page=1

 

[tomstickland]

The link describes my previous method of doing this.
At least it will pick up the diameter if it ever changes, but the pitch information will need manual editing. I want the drafting package to automatically update if the thread ever gets changed.

 

[tomstickland]

It turns out that you can easily add fully parametric thread size leaders to drawings.

Do "insert-Feature Parameters".
Expand the list until you find the parameter of interest, eg: Threaded hole 4.
The relevant feature on the drawing will highlight.
Pick the view where you want to place the leader.
In the top right of the window pick "ansi_mm" from the drop down list.
OK the operation.

This then places a draggable leader on the drawing with both the thread diameter and pitch on it.