Convert model to Fine Tolerance

[Julian Marchitti]

Hi,
I've been modelling Compressor Blades and Vanes in NX12 for a few months now, and I've used the Standard Model Template. I had a conversation last week with a colleague in Siemens Montreal, and he informs me that I should be using the Fine Tolerance Model. Apparently, the FEA package (SC03) used to analyse the models operates on very fine tolerances, and if a standard tolerance is used, the surfaces do not meet.

Assuming this is true, can anyone tell me how I can retrospectively change to a Fine Tolerance Model?

Thank you!
Julian

 

[RX8UK]

Hi Julian,

I'm not sure what you mean by "Fine Tolerance Model". Is this a local template new part?

Tolerances can be set in Menureferences:Modeling.

If you had the distance tolerance set to say 0.01, you cant just change this to 0.0001 and all the feature operations update. You would have to go through each and change the tolerance.

I'd probably start at the first feature and used edit with rollback and work through the model. This could be automated I guess.

I hope this helps.

Regards,

Paul

 

[jerry1423]

You can try going thru your model starting with the first feature and then tighten the tolerance on that feature then each feature down the tree. To see the tolerance of the feature you may need to expand everything in the menu. It should be under "settings".
If this is a fully surfaced model then you may just want to edit the feature of the surfaces in the model tree and tighten those tolerances.

Jerry J.
UGV5-NX1884

 

[JohnRBaker]

Paul and Jerry are correct, while you can change the default model tolerance of a part file, this change will have NO effect on any of the existing features. You will need to edit each one of them if you wish them to use a smaller tolerance value. Now if there are a large number of features and/or a large number of part files which you needed to 'update', you could write a small program that would cycle through the features, editing the tolerance value for each one.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[Toost]

I am not so sure about the requirements here, you should check that before doing anything.
FEA(FEM) systems generally work with , In the CAD perspective, quite crude tolerances, the FEM result is a form of approximation.
I have seen a number of cases, at different companies, where the designer was instructed to create surfaces w very tight tolerances to points, points that was exported from a FEM simulation.
the problem was that the imported coordinates only had one or two decimals ( that was the accuracy of the FEM simulation), and when the designer in NX used these points , he/she was required to include all points to a specific tolerance, the result is/was an unusable surface. wobbly/wavy/not smooth/unusable and often extremely heavy.
I have a part file from one of these examples. it contains the outer shape of a wind turbine wing, one sheet body w two faces. Nothing else in the part file. +6.5 Mb and completely unusable.
But, that said, you might have a common methodology within your company where the NX models should be using a specified tolerance etc.

Regards,
Tomas

 

[Julian Marchitti]

Thank you all for you replies.
Sorry I wasn't more specific Paul. Yes, Fine Tolerance Model is a template. When creating a new model, we are given a choice of two templates, Standard Model and Fine Tolerance Model. I have always used Standard Model, but I'm told it's better to use Fine Tolerance Model when creating parts for analysis. I'm not sure how much difference it actually makes!

The aerofoils are defined by some very old microfilm drawings (1950s in most cases) called CBF (Compressor Blade Files). Numeric tables of XY coordinates define a 2d aerofoil profile at given sections. We create a sketch on that section, and create a point for each XY coordinte. A Studio Spline is created through the points, and a surface is then created through the Studio Splines from all the different sections. I have to admit that the surfaces are often quite rough, and we have to open up the tolerance just to get them to sew into a solid. I suspect this ties in with Jerry's point. If we encounter a problem, I suspect we may have to improve the quality of the surfaces so that we can sew with a tighter tolerance.

John, I would be very interested in having a go at creating a program to tighten the tolerances, but I wouldn't know where to start. Would you be able to get me going or give me an example, please? This is probably more for my own interest than anything else, so please don't go to too much trouble!

Thanks again,
Julian

 

[JohnRBaker]

I'm sorry, but I retired over four years ago and no longer have access to NX. I'm sure that there are others here who could help you get started.

John R. Baker, P.E. (ret)
EX-Product 'Evangelist'
Irvine, CA
Siemens PLM:
UG/NX Museum:

The secret of life is not finding someone to live with
It's finding someone you can't live without

 

[jerry1423]

Wow, it's been four years already !

Jerry J.
UGV5-NX1884

 

[cowski]

Some code was posted a while back in the Siemens community forum that might help you.

https://community.sw.siemens.com/s/...E/automating-the-update-of-modeling-tolerance

www.nxjournaling.com