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NX 7.5 Distance Tolerance Setting

Pioneer
Pioneer

Hi,

 

I would like to set default distance tolerance from 0.0254mm to 0.001mm so that each time I open new file it will follow 0.001mm.

 

I have set the Tolerances / scales in Customer defaults to 0.001mm as per below :

 

7.5.png

 

However , in the modeling preference ; the distance tolerance is still set to 0.0254.

 

7.5_2.png

 

So each time I need to change the distance tolerance to 0.001 in modeling preferences.

 

However , the Bridge curve distance tolerance setting is still 0.0254.

 

May I know how do I preset the distance tolerance to 0.001 , each I open a new file ?

 

What is the difference / effects between the tolerance settings in Customer default and modeling preferences ?

 

Thanks.

 

Jerman

4 REPLIES 4
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Re: NX 7.5 Distance Tolerance Setting

Siemens Valued Contributor Siemens Valued Contributor
Siemens Valued Contributor

Hi @jerman -san,

 

The customer defaults scope is PART.

Please refer to the picture.

“0.0254” is stored in the template part selected when creating a new template.

 

>>What is the difference / effects between the tolerance settings in Customer default and modeling preferences ?

Same preferences.

However, since the range is PART, the value of the template part takes precedence unless it is created with blanks.

 

>>May I know how do I preset the distance tolerance to 0.001 , each I open a new file ?

For example, when using a "Model" template, edit the template file.

If you select "Blank" when creating a new, even if the range is PART, it will be inherited from the customer default.

 

 

The following is an example of editing the Model template part (metric).

 

1) Backup template part

       Location: %UGII_BASE_DIR%\UGII\templates

       File Name: model-plain-1-mm-template.prt

 

2) Open model-plain-1-mm-template.prt

3) Edit Modeling Preferences

4) Save and Close part

 

Best Regards,

Seiji

Re: NX 7.5 Distance Tolerance Setting

Pioneer
Pioneer

Hi Seiji ,

 

Thanks for input , I manage to change the distance tolerance to 0.001 from the template file.

 

Now , opening new file inherent the setting , however , I find the bridge curve distance tolerance is still 0.0254 ;

 

I thought it should follow the setting on the modeling preference.

 

It there any way to preset to 0.001 ? Or I have to set it manually ?

 

Thanks.

 

Jerman

Re: NX 7.5 Distance Tolerance Setting

Gears Phenom Gears Phenom
Gears Phenom

You have to follow the @Seiji 's steps as I show in the movie.

 

(view in My Videos)

Re: NX 7.5 Distance Tolerance Setting

Siemens Valued Contributor Siemens Valued Contributor
Siemens Valued Contributor

@jerman -san

Sorry for the late contact.

I had a long vacation.

 

> Now , opening new file inherent the setting , however , I find the bridge curve distance tolerance is still 0.0254 ;

> I thought it should follow the setting on the modeling preference.

> It there any way to preset to 0.001 ? Or I have to set it manually ?

 

It is the dialog memory value recorded before editing the template.

Click the reset button at the top of the bridge curve command dialog.

For part settings, the reset value is inherited from the part settings.

 

 

@Cesare -san

Thank you for your clear follow-up.