Nx 10 Dimensions Becoming Disassociated with Templates created in Nx 8.5

[Nick66]

Hello, I created templates in Nx 8.5. The dimensions are controlled by inputting different values in attributes. They work normally in Nx 8.5, but now that we are using Nx 10, there are many times where the dimensions are becoming disassociated after the changes are applied in attributes. Is this normal for Nx 10? Is there a default which I can change? I have attached the file saved in 8.5

 

[cowski]

I opened your part in both NX 8.5 and NX 10. From my very limited testing, it seems to behave the same in both versions. If I switch to the drafting application and change the cutter diameter (Dc), the views update as expected. Changing the overall length (l2), causes the view to go out of date and requires a manual "update view" operation. This is strange because "automatic update" is turned on in the preferences. However, starting from the modeling application and making changes updates the model; switching to the drafting application, the views update and dimensions are correct no matter which parameter was modified.

I only did a little bit of testing and only minor changes to the existing values. I didn't see any dimensions become disassociated; are there combinations of values that are causing errors?

www.nxjournaling.com

 

[Nick66]

Cowski, the value for the l2 is multiplied by 4.25" to determine the scale of the view. I'm not sure if that is why you need to manually update, but I have thought the same thing you did about that. If you change an individual attribute, you are right, it seems to work fine, but it is when you are changing multiple that it has the issue. Could you please try to input these values and then apply?
ap: .250
Dc: .125
dmm: .250
Dn: .173
l2: 2.000
l3: .750

 

[cowski]

Ok, I see the issue now. I don't know the root cause for the dimensions becoming disassociated, but I tried recreating the view using the newer "exact" representation (as opposed to the "Exact (Pre-NX8.5)" type) and the dimensions updated as expected. I'd suggest raising the issue with GTAC so they can investigate; it seems there is some lost functionality somewhere between the releases.

www.nxjournaling.com

 

[Nick66]

I'm not sure what you mean by this "I tried recreating the view using the newer "exact" representation (as opposed to the "Exact (Pre-NX8.5)" type)" and how does one bring an issue up to GTAC?

 

[cowski]

When you place a base view on the drawing, you can open the settings and choose the representation type. This must be done before placing the view, the representation type cannot be changed after the view is placed.

To report an issue with the developers, you go through your reseller or directly through GTAC. You will need to be up to date on maintenance payments and have a webkey account set up (your company probably already has one set up). After that, you can log an incident report (IR) by calling GTAC or filling out an online form (NX menu -> help -> online technical support -> log an incident with technical support).

www.nxjournaling.com

 

[cowski]

There was supposed to be a screenshot in my previous post, but it didn't come through for some reason. I'll try to attach it to this post rather than embedding it.

www.nxjournaling.com

 

[Nick66]

Thank you for your help today Cowski