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Use Tolerances from Part in Drawing

10 REPLIES 10
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Message 1 of 11
JMoore-OF
3936 Views, 10 Replies

Use Tolerances from Part in Drawing

Hey Guys!

 

I set up default tolerances in my part and would like to have them displayed in the drawing.  I used the "Retrieve Dimensions" tool but they aren't showing up.  I have the Tolerance Method set to Default.  Any idea what i'm doing wrong?

 

Thanks in advance!

10 REPLIES 10
Message 2 of 11
mcgyvr
in reply to: JMoore-OF

Open idw template..manage tab..styles editor.. click on your dimension style.. go to the notes and leaders tab... click the precision and tolerance button. check "use part tolerance". save style, save template

Have fun 🙂



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Message 3 of 11
jletcher
in reply to: JMoore-OF

If you are in 2012 there is a bug and it will work when it wants to. I have this issue with most of my clients and it is very frustrating.

 

Message 4 of 11
JMoore-OF
in reply to: JMoore-OF

@

Message 5 of 11
jletcher
in reply to: JMoore-OF

LOL really you sure they fixed the bug haha that's funny.

 

Please list the version next time if you don't mind hard to help if you don't know the version

 

Best of luck

Message 6 of 11
JMoore-OF
in reply to: JMoore-OF

Sorry for not posting the version off the bat...

 

I had been using the default tolerance setting from "Document Settings".  The tolerances appeared to be fine in the sketches in the part but did not appear in the drawing.  However, when I created custom tolerances for each dimension in the sketch, they show up perfectly in the drawing.  What am I missing here?

Message 7 of 11
karthur1
in reply to: JMoore-OF

There are a few things you have to do to make this work  I am using 2013, so it might be a little differnt in 2014.

 

1. In the part, set the tolerance that you want..obviously.  You can apply a global tolerance (like you have done) or on a "per dimension" basis.  If you are after a global tolerance, you "could" handle that with a general note on the idw.

2. Also in the sketch, change the Dimension Display to "Tolerance".

3. In the idw, go to Styles Editor.  Set the default tolerance close to what style you want your toleranced dim to be. You cant set the default to Frac and then change it to decimal later. If you dont, it wont work.  Your default tolerance dim should be the same type as what you want to end up with.... For example. Say you have a fractional style and a 3plc dim style and you set the frac style as the default for a linear dimension.  Next you retrieve the dim in the idw and the dim is placed as a frac style.  Now when you change it to 3plc to see the tolerance, the tolerance will be lost.  Mine always shows ".000"  You could set the default to a 1plc, 2plc, 3 plc or 4 plc...etc and it would work.

4. Once you have this set, right click on the view and choose "Retrieve Dimension" and pick the dim that you want.  The tolerance should show.

 

A few caveats:

1.  Later, if/when you decide to change the tolerance of the model, open the sketch and change it there. DONT leave the visibility of the sketch on and change it without being inside the sketch.  If you do,  The idw WILL NOT update.  I learned this lesson the hard way.

2.  If you chagne the tolerance in the part and then go back to the idw and get a message "The following components referenced by this drawing need to be updated..."  (if its not suppressed), then you did something wrong.  You will not get this if you edit the tolerance from inside the sketch.

 

Kirk

 

Message 8 of 11
karthur1
in reply to: karthur1

One other thing,  When you set the tolerance in the part... if you sue the "Default" Tolerance type, then the tolerance will not shown on the idw.  I usually use the "Deviation" type" even if it is symmetrical.

 

2013-07-12_0915.png

Message 9 of 11
Anonymous
in reply to: JMoore-OF

Check this:

In document setting, default tolerance tab, Use standard tolerancing values is checked.

In the idw you can right click the dimension, edit model dimension, click the arrow to the right of the dimension and change the number of decimal places on the tolerance.

The tolerance should then display in the idw according to how you have it setup in the default tolerance setting.

Message 10 of 11
karthur1
in reply to: Anonymous

I just learned something, thanks John R.  From my Note 2 above where I said to set the default dim to be similar to what you want.... disregard that.  You can leave it set to what ever you want by doing it this way.

 

1. In idw, retrieve dimension. Change it to the format you want Annotate>Format panel.

2. Right click on the dim and chose "Edit Model Dimension". Change the Tolerance type to Deviation (something other than Default). Voila.... the tolerance now appears.  You can even edit the Tolerance value and it updates the model and the part to match.

Message 11 of 11
Anonymous
in reply to: karthur1

You can leave the model tolerance set to default, as long as you change the precision on the model tolerance to match the tolerance for the number of decimal places you have setup in the default tolerance table in document settings (in the model).

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