NX - Edge Blends / Fillets seem to bog / slow model down - Suggestions?

[Ryan68sports]

First time poster, long time reader here.

I absolutely love NX, but I have one thing that keeps creeping up.

On several different part models I have worked on, each around 1,000 features/part navigator/tree items, it seems that when I get to the end and start adding Edge Blends (fillets) that the model just gets slower and slower. After several fillets (most are variable radius as part changes size/shape) it may take several minutes (maybe as long as 5 to 15 sometimes) to go back in edit these fillets or add new ones (Mainly seems to be on editing existing ones though). Taking preview off does help speed this up but then if you click ok to save changes then your wait begins. Gets frustrating after awhile. You see the end in sight with the last few touches but it may take you all day or more to finish.

I haven't seen anyone else talk about this so just wondering if just a setting change somewhere possibly or my computer hardware / software compatibility? When NX is churning away thinking, Windows task manager says I'm not even using 25% of my ram and barely any CPU.

NX works great otherwise.

Any thoughts/suggestions/links to other post appreciated.

Thanks,

NX 7.5 and 9 (better performance in 9)

PC:
Dell Precision T5500
Intel Xeon CPU - E5645, 2.40 Ghz , 2.39 Ghz (2 processors)
12gb RAM
64-bit
Windows 7

 

[JohnRBaker]

What Distance and Angle tolerances are you using (check Preferences -> Modeling...)?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ryan68sports]

Dist: 0.0004
Angle: 0.5

I have 3 or 4 times set feature to 0.0001 to get a feature to Sew together before (if that makes a difference).

 

[JohnRBaker]

Are you working in Metric or Imperial units? And about how large, physically, are your typical models?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ryan68sports]

Inch units.
Typically part file is maybe around 40mb before drafts/fillets are added...around 100mb after.

 

[JohnRBaker]

When I said physically, I meant SIZE in terms of how big is it in feet and inches.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Ryan68sports]

Whoops!...was going with physical file size there....

Pretty small, but a lot of features placed on it. this part may be around one foot tall, Less then three inches thick.

 

[JohnRBaker]

Your tolerance values look about right, in fact, you're using what the new out-of-the-box default Distance tolerance is now set to for NX 10.0 (which was changed from NX 9.0 and older versions of UG/NX). Typically how many different blend feature do you have versus the total number of features? Is the rest of the model simple shapes or mostly freeform faces? If they are freeform faces, how were the original shapes creaetd, as surfaces sewn together or some other technique, like using a surface to trim away a larger solid 'block'?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[jerry1423]

or replace face from a solid block ?

Jerry J.
Milwaukee Electric Tool

http://www.milwaukeetool.com/

 

[Ryan68sports]

Typically end up with around 30-40 or so Edge Blend features, placed at the end of say 1,000 items in the part navigator. Several edge blends are variable radius to work with the thinning/curving surface of the part.

Initially we start off by creating a solid body by trimming reference boundaries(surfaces) and then sew that into a solid body. That lets us then do the 'easier' stuff (trims/cuts, slots, holes, etc.) through the built in feature and sketch tools as applicable. We also though have areas of the part where its created one area at a time, as it involves different final needed shapes in different areas (maybe creating a curving tube that keeps changing shape as it winds through the part here or there, etc). These sections, if you will, of the part are created using reference surfaces/bodies from WAVE geometry, ref planes, or other geometry to set up some of the known boundaries, then sketches/extrudes and/or surfaces (offset surfaces, surfaces created with curve geometry, through curves, sweep, etc) make up the rest of the feature generally (usually find a lot of Trim and Extend, Trimmed Surface, N-Sided Surface commands), followed by sewing that feature area together, then Unite it with the rest of the part. After uniting the final parts of the model together we apply drafts followed by the edge blends and we're done.

Hope I answered your questions there.

Since you mentioned it, I'll take a look at NX 10 to see what's new. Always curious on what new toys have been added.

 

[Ryan68sports]

Just played around with some of the Facet Settings which improved performance with the fillets a fair amount.

 

[JohnRBaker]

OK, so that indicates that it's might not be the modeling execution that is impacting your observed performance but rather the display of the model that is having a significant impact. As a test, not really a recommended way to work, before adding one of those final blends to your model, change your 'Rendering Style' to 'Static Wireframe' and see what impact this has on the time to complete the operation. 'Static Wireframe' is about a basic as you can get in terms of what it takes, software/hardware wise, to display your model.

Anyway, if you do give this a test, please let us know what you learn.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.