Customising the Material Database

[rossob]

Is anyone able to offer any help as to the best practice for modifying the material database? I want to try and add company-specific material descriptions to assign to parts, which can also be linked to drawing attributes.

I have modified the PHYS_MATERIAL.DAT file and have copied the line for STEEL to an unused line and renamed it to 6mm 250 GRADE PLATE. However the new material never appears in the database when i re-start NX.

Am i doing something wrong, or is there a better way to do this?

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[JohnRBaker]

I don't know. It worked for me. Make sure that you actually replaced the existing file since it's stored in a 'read-only' state.

Also make sure that you assigned your new material a unique 'libref' number (first field of each material record).

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[Kirsten]

I found in NX2 that it didn't like having spaces in the names, and that it was limited to a certain amount of characters (31 is too long).

John,

If I insert new materials in the middle of the list such that the libref number for Brass, for example, changes from 26 to 27, will I be creating a problem in a part that already had that assigned? I wanted to put them in alphabetical order...

 

[NXdesigner]

We are looking at using NXNastran for our FEA analysis. Does NXNastran use this user defined NX material database or is there a prepopulated database that comes with NXNastran? I find it hard to believe that I will have to populate this database to use NXNastran.

 

[JohnRBaker]

Kirsten,

I don't know as I never tried that. While the 'libref' number is unique in the file, I don't think it matters since the material if 'loaded' into the part file where it becomes it's own record there and that's why if you go back to the Material tool once you've assigned a material previously you will see that it's been 'loaded' into a registry on the top-level dialog where it can be accessed again if needed. In fact you could bring several materials up into the part file and then use the Material dialog to more easily access them when needed, perhaps if you were conducting a series of tests and needed to go back and forth between several different materials.

NXdesigner,

This material database was provided to use by the CAE group as the whole material assignment function was developed explicily to meet their needs. The user Attribute and model density was only seen as secondary functionality.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[rossob]

John/Kirsten,

Thank you for your replies. Kirsten, NX5 doesn't seem to like spaces in the material name either.

My next question is now that i have assigned a material to my component, is there a physical attribute address somewhere i can use to link a drawing note to?? ie. <W@$SH_SHEET_SCALE>

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[rossob]

Sorry, also forgot to add something to that last post.

Because there has to be underscores in between words in the material name, this description is useless to use on a drawing. Is there a useable description that can be assigned to these material names?

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[Kirsten]

I did find out that if I set the customer default "Gateway>General>Update material properties from library on part load" to yes, and if I renumbered the materials in the library, that I will get a message while working in the part that the assigned material properties have changed, do I want to update? If I then hit the button to update the material in the part, the material and material attribute will change.

 

[hudson888]

This interests me.
I do like a good customization and many people would do too. Can anybody tell us what the material attribute is called that you're using. i.e. going back to Ross question as to whether there is something that can be plugged into <W@MATL>, or <W@$MATL> to maintain a note on the drawing. I know how to use it to maintain the masses but these are assigned to bodies not parts and there doesn't seem to be any resultant attribute anywhere that I can obtain to put the material on the drawing.

If there is I'd be happy to hear of it. Otherwise NX-6?

Best Regards

Hudson

 

[JohnRBaker]

The Material 'Attribute' can be defined in Customer Defaults -> Gateway -> General -> Attributes.


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[hudson888]

Well done John.

I see that it is a new thing for NX-5 that I hadn't caught up on.

Best Regards

Hudson

 

[rossob]

Hi John,

thanks again for you reply. I did realise that the Material 'Attribute' can be defined in Customer Defaults -> Gateway -> General -> Attributes, however, I am still a little unsure of linking to this property.

When you highlight the information symbol at the above customer default you get the following message: "This option specifies whether or not a Part Attribute will be created and/or updated to reflect the current Part Material." There is a field underneath that which is where you define what the attribute is, as a default it is MATERIAL. However I couldn't find an attribute called MATERIAL anywhere that had been created.

I could manually enter in a material attribute, assign a material description, and then link to that property in a drawing. This is a workaround, but not really linking to the material selected from the material database. Is that material accessible anywhere, or is it only really to be used for, say, mass properties or C of G properties?

I have worked out how to link notes on drawings to properties via the <W@$SH_SHEET_SCALE> etc, but was wondering if there was a list of these global part properties/attributes available anywhere to view? ie material thickness (sheet-metal part)

Thanks again in advance for any help you may be able to offer.



Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[JohnRBaker]

First thing to understand is that the Customer Default setting does not actually cause any attributes to be created, that only happens if and when you assign a material to one or more solid bodies in your part file.

Now when you do assign a material (BTW, there are 2 places to assign a material in NX but these attributes only work with the item found under Tools -> Materials Properties...) if you had set up both Attribute options in Customer Defaults, then a Part Attribute will be assigned to the Part File and an Object Attribute will be assigned to the Solid Body that was selected (note that if there are more than one Solid Body in the Part file and you've assigned different materials to each Solid Body, the nmae of the LAST material assigned will the one that the Part Attribute will carry).

Now when it comes time to create a drawing of say an assembly where the various parts have been assigned material properties, the actual Attributes read by the Parts List code are the Object Attributes assigned to the Components in the Assembly. When a Part is added to an Assembly as a Component, the Part Attributes of the Part file get assigned as Object Attributes on the Components.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[Dave K]

Does the "part attribute" and the "object attribute", have to be different? We're not using them yet, but I noticed they are both "Material" right now.

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[JohnRBaker]

No, they can have the same name since they are two different types of attributes (no where does any NX application look are both types in one operation so a common name will not cause confusion).


John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[rossob]

John,

I was able to get that working fine, didn't realise you had to select the part body before assigning a material. I thought you could just assign a material to the entire part. Once this material was assigned, I was also able to modify the description to remove the underscores.

Many thanks.

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[JohnRBaker]

I'm glad we finally got you on the right road.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

 

[rossob]

Yes, thank you for your help, it is very much appreciated. I am a relatively new user, coming across from 6-7 yrs of Solidworks, and have been very frustrated knowing what i want to do, but not being able to make certain things work.

The next question I have now relating to the above, is relating to drawings. If I add a drawing sheet to the existing part, I can link a note to that MATERIAL property easily, by selecting Edit Text => Relationships => Part Attribute.

However, if I created a separate blank drawing and added a drawing view of, say a sheet-metal part with an assigned material I can't seem to link to it. IF i right-click that component in the Assembly Navigator and check its properties, there is an attribute there now relating to it's material. The problem i am having is linking a note to reference that property.

Anyone able to offer any advice, or point me to anywhere i may be going wrong??

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007

 

[hudson888]

I just caught up with this thread and found the time to check it out. This is a big step forward in my book because previously you could always assign the density via the material properties, but we used it all too seldom since the attribute used for the drawing still needed manual input. Now that you get both it really justifies creating and maintaining a materials database. Now if only we could get rid of those darned underscores then it would be perfect.

Cheers

Hudson

 

[rossob]

Hudson,

I agree, a company-specific materials database is a big time-saver, and also ensures that each designer is using the same material descriptions in the same formats, spelling, abbreviations, etc.

I found that you could assign the material to the part, and then manually remove the underscores from the description. It's a work-around, but it's a start

Ross

NX5.0.2.2 WinXP SP2
SolidWorks 2007