Flat Pattern adding to mass

[Jackrabbit49er]

We are running NX 8.0.3.4 and I am noticing that on some parts the flat pattern is adding to the automatically calculated mass of the part. The body measurement is no affected by the flat pattern. Has anyone else come across this?

Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[JohnRBaker]

I just tested NX 8.0.3.4 and I can't duplicate that behavior.

Now when you say "automatically calculated mass of the part" where are you observing this value?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
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[Jackrabbit49er]

Mr. Baker:

The automatically calculated mass I am talking about is on the weight tab of the displayed part properties dialog box.


Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[cowski]

From the NX help file (analyze assembly -> advanced weight management):

Calculating weight for a subset of bodies
By default, weight properties are calculated based on the entire assembly or part. Hidden solid bodies and solid bodies on invisible layers are included. If you want to use only some of the solid bodies, you do so in one of these ways:
[ul]
[li]Change the work part to a lower level in the assembly, and then choose Work Part in the Weight Management dialog box for the properties of the work part and its components.
[/li]
[li]Choose a reference set or a component group to define the solid bodies used in the calculations.[/li]
[li]Or choose Selected Components and select the components whose weight properties you want to calculate.[/li]
[/ul]

www.nxjournaling.com

 

[JohnRBaker]

That's what I tested. Now you mentioned that this only was apparent in some of the parts so you need to check this out.

The Properties weight information is only measuring what the system finds in the 'Model' Reference Set. Now under normal conditions the flattened solid is NOT added to the 'Model' Reference Set as it gets it's own dedicated Reference Set, however someone may have edited the 'Model' Reference Set to explicitly include the flattened solid for some reason so you may wish to check that for those parts which are not giving you what you expected the proper weight to be.

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

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

 

[Jackrabbit49er]

Mr. Baker:

I do not have a flatten solid in the part. It is only a flat pattern.

Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[cowski]

Check to see if you have any solid bodies that are hidden or on other layers. They can add to the mass, curves from a flat pattern cannot.

www.nxjournaling.com

 

[Jackrabbit49er]

Cowski - I agree that a flat pattern shouldn't, that is why I am flabbergasted. Supressing the flat pattern will return the mass to the same value from the measured body feature.

Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[JohnRBaker]

When you create a Flat Pattern, a Flattened Solid is created first and then it's edges are extracted to get the 2D set of curves which make up the Flat Pattern. This body is NOT removed from the model but rather it's 'managed' in such a way that it can be assumed to no longer exist. That being said, this 'hidden' ('managed') Flattened Solid CAN BE made visible and accessible by selecting the 'Flat Pattern' feature, pressing MB3 and picking the 'Make Flat Solid External' option. Once exposed as it's own feature it could be manually added to the 'Model' Reference Set and then moved to another layer or something. However, if while the Flat Solid was 'external' you did add it to the 'Model' Reference Set and then you make it 'internal' again, the system is smart enough to set the Properties Weight back to the correct value as if it were no longer part of the 'Model' Reference Set.

Perhaps if you uploaded one of the 'problem' parts we could look at it and see if we could solve the mystery.

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

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

 

[Jackrabbit49er]

Mr. Baker:

The Model reference set has 1 object while the Flat_Solid reference has two. If I remove the flat pattern, the flat_solid reference becomes empty. Any thoughts?

Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[JohnRBaker]

I'm not surpised, but without seeing your actual part file there's not much more that I can comment on.

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

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

 

[cowski]

By how much is the flat pattern changing the weight value?

www.nxjournaling.com

 

[Jackrabbit49er]

Mr. Baker - My CADadmin has opened IR 6859896 with the file. He has indicated you will be able to get to this.

cowski - the flat pattern is multipling the mass by a factor of approximately 3.

Why do you have to be a nonconformist like everybody else?
- James Thurber

 

[looslib]

It should be about double if it really is the flatpattern solid causing this.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

I'm sorry, but files submitted through GTAC for an IR/PR are only accessible by those Siemens PLM employees authorized to work on customer parts (which I'm not since I don't write or modify code nor work for GTAC). So if you don't post a sample here, there's no way for me to access the files you've sent to us.

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

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

 

[cubalibre000]

Hi Jack, l had the same problem and only on sheet metal parts. Parts with problem came from NX7 and after a refile process. Not all sheet metal parts had this problem. The problem is located on which reference set NX uses to calculate the weight. On those parts, the reference set used, it was erroney 'entire part', while the correct it's 'model'. If you have 'weight management' license, you can correct the problem.

Thank you...

Using NX 8 and TC9.1