Chamfer Dimension Display in Drawings

[Joest]

All,

Maybe this is a bug, or I could just be doing something wrong, but when I ask SW2005 to display a chamfer dimension in the, for example, 1X45deg format it does not do it. It typically displays the size and the angle as two seperate dimensions which is quite annoying. Any solution will be greatly appreciated.

Thanks,

Joest

 

[ctopher]

What do you mean in two separate dimensions. Can you display how you see it?

 

[Joest]

The angle is a seperate dimension with its own leader and the length is as well. Ideally, a chamfer dimension would tie the size and angle information together and they would have a common leader. Does this make sense?

 

[TheTick]

Sometimes, I make a custom property that reads the two chamfer dimensions in the part. In the drawing, I attach a note to the chamfer that references the custom property. Works for slot notes, too.

 

[Joest]

Tick,

Could you give an example of what your inputs are within the note? I've tried to do this using the dimension ID, but haven't got it to work yet. Back in my ProE days this was used all over a drawing.

Aside from you method, I would still like to know why SW will not display chamfers this way even when I select it in the "document Properties" menu.

Cheers,

Joest

 

[mncad]

Joest,

I'm not sure why your SW2005 is doing chamfers that way. I just tried it in SW2005 SP0.0 and it worked just fine, had it all off of 1 leader. Might check the settings in the file.

mncad

 

[jhricm]

Joest,

These settings change the display of chamfer dimensions added to the drawing with the chamfer dimension command. I do not believe that it will change the display of those that are imported into the drawing from you part.

Jim

 

[SBaugh]

Have you looked @ Tools\Options\Document Properties\Detailing\Dimensions\Leaders ? - There you can customize or override the Chamfer standard leader display. This also probably resides due to the fact of what Standard you are running. WHat standard are you running?

mncad - What standard are you running so we can compare it to what Joest is running. Of course Joest you will need to post your standard.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[imagitec]

Joest,

Does the problem occur when SolidWorks automatically creates the dimensions from the model? If so, you may want to insert the chamfer dimensions manually via Tools->Dimensions->Chamfer.


Rob Campbell, PE
Finite Monkeys -

http://www.livejournal.com/users/robcampbell

 

[mncad]

Scott,

I'm using the ANSI standard, and I did create the chamfer dimension in the drawing, I didn't import the dimension from the model, when I import the dimension it gives the dimension and the angle separately as dimensions, not as leaders as the tools->dimensions->chamfers does. Another way to access this is with a RMB when you are in the dimension command, pick "More Dimensions" and chamfer is the last in the list.
mncad

 

[ctopher]

I don't understand exactly how you created the dim, but try the chamfer dim icon, select the angle then the straight line, place the dim.

 

[Joest]

It looks like the problem is solved. I followed rjcjr9's advice and created the dim in the drawing with the chamfer command and it displayed correctly. It's unfortunate that imported dims must not follow the rules a user specifies in the document preferences. I would venture out and say this is a bug that should be corrected.

In an earlier thread, TheTick mentioned how he places parametric values into his notes that automatically update. How is this done exactly. What is the nomenclature used within a note to have values read in? I have already tried using the dimension names that are given when the dim's properties are viewed (example: RD1@drawing view4 of test hub) but must not have my syntax correct.

 

[MElam]

To place parametric values in notes:
While editing the note, place your cursor where you want the linked dimension and then go select the dimension from elsewhere on the sheet. It will place the proper syntax for you.