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How to make tolerance to be added automatically from model into the Hole Table?

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hello,

 

I created three similar Simple Screw Holes which differ only in "Fit" Parameter:

FIT.png

 

I want these three "Fit" values to be present in the Hole Table next to the diameter here:

fit4.png

How to make NX to place these values in the Hole Table automatically? 

5 REPLIES 5

Re: How to make tolerance to be added automatically from model into the Hole Table?

Gears Phenom Gears Phenom
Gears Phenom
@Lidia,

Look under Preferences -> Drafting then scroll down to the the Table node and expand it so that you see Hole Table. Expand the Hole Table node and select Content. Check the Diameter Fit box.

NX12 Docs link:

https://docs.plm.automation.siemens.com/tdoc/nx/12/nx_help/#uid:xid1128417:index_drafting:id700849:x...
Tim
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1

Re: How to make tolerance to be added automatically from model into the Hole Table?

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

@TimF ,

 

I have the Diameter Fit check box on, but the column named "Diameter Fit" is still empty.
fit5.png

Re: How to make tolerance to be added automatically from model into the Hole Table?

Gears Phenom Gears Phenom
Gears Phenom

@Lidia,

 

This can get a bit complicated - if you read the link I posted in the Diameter Fit area, there are some key things mentioned.

 

First, your Drafting Standard has to be set up correctly. (Customer Defaults -> Drafting node -> General/Setup) (Go to the Standard tab and then click on Customize Standard -> under Table node check both the Content tab - you want to make sure the Diameter Fit is checked - and next the Attributes tab needs to have the Diameter fit area defined with at least "D_TOL").

 

That should make sure all new drawings will allow for this Hole Table to display info as you wish (hope this makes sense). If all of this is set, we should be good to go.

 

From this point forward, we are simply focusing on your original question.  The above is to make sure NEW parts and drawings will work as you expect (for the fit tolerance only - read the docs for the rest, it's very similar).

 

So, go over to your model and select the face of the hole feature.  You want to make sure NX has the feature and not just the face (the Quick Pick should show you this - Face of Simple Screw Hole.....).  Once you have the feature face selected, right click and choose Properties.  Select the Attributes tab and for Title/Alias enter "D_TOL" (no quotes).  Under Data Type, select the Expression Formula button (left side) then for Expression Formula, go to the right side and the pulldown where the double quotes should now be, use the pulldown and select Reference -> Feature Parameter.  Click the Hole and then click the expression for the Fit tolerance from the list of the parameters that pop up.  Click OK then back to the Face Properties dialog either click the green check box, Apply or OK.  You have now created an Expression for the Hole face that is (and always will be) equal to the Fit tolerance expression value.

 

Now go over to your drawing, update the Hole Table (from the Part Navigator) and your Fit Diameter tolerance should display in both the fit column and next to the hole description.

 

After going through this, I guess you can turn off the column via Drafting Prefs.  The important part is the Attribute for the hole face.

Tim
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1

Re: How to make tolerance to be added automatically from model into the Hole Table?

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

@TimF  Thank you very, very much! That works! You made my weekend!
solution.png



Re: How to make tolerance to be added automatically from model into the Hole Table?

Gears Phenom Gears Phenom
Gears Phenom
@Lidia,

Glad I could be of some help. Have a good weekend.
Tim
NX 11.0.2.7 MP11 Rev. A
GM TcE v11.2.3.1
GM GPDL v11-A.3.5.1