Callouts for material, quantity and sheet metal preferences?

[Ritchie]

Hello NX community,

I'm working on an assembly made out of several sheetmetal components. I use the master model approach to make individual drawings of these parts. I would like to have as much information as possbile "automated" in the drawing file. I wonder if and how it would be possible to show the following information in the drawing:

- Material of the referenced part
- Weight of the referenced part
- Quantity of the part in the master assembly
- K-factor (neutral factor) of the referenced sheetmetal part
- Bend radius of the referenced sheetmetal part
- Thickness of the referenced sheetmetal part

I know these last two items can also be pointed out by means of measurements, but it would be nice to be able to show this information in a table on the drawing as well.

If you know the answer to any of these questions it would be very appreciated if you can post the relevant call outs as well!

Thanks in advance!

 

[Ritchie]

By the way, I'm on a stand alone NX 8.5

 

[JohnRBaker]

Have you set up Parts List in your Assembly Drawing?

Are you assigning material using the Tools -> Materials -> Assign Materials.. function to assign materials?

As for the K-factor, minimum bend radius and the material thickness, these values are all recorded as Expressions in the part files created using the NX Sheet Metal module.

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.

 

[Ritchie]

Thanks for your reply John...

Yes, I have set up a parts list in my assembly drawing.

Yes, I'm using Tools>Materials>Assign materials to assign materials to the parts.

Is it possible to display these sheet metal expressions in the drawing? If so, how? Expressions are different from part attributes, right?

 

[KhimaniMohiki]

To get the component expression in an assembly parts list:

In each of the components create a new attribute for each of the expression you wish to see in the drawing, link the expressions to the attrubutes using Link to Expression from within the attribute dialog.

Then in your assembly drawing you can call these attributes into the parts list.

To get the expressions in the component drawings:

Create a table, exnter the expression in the table in the format <X@pxxxx> where xxx represents your expression number. You can also edit the table using a spreadsheet then under the Add-Ins tab Import NX Expressions

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[Ritchie]

Thanks all for replying. I still can't get it to work though. I have managed to get the material and the revision of the dummy part displayed on the drawing, but there seems to be no way to get the weight displayed on the drawing.

When I open the dummy part, File properties there is a listing for "Masspropmass".

When I want to add this value to the drawing template (Relationships>Object attribute) there is no listing of this value. There are values for Material and revision (DB_PART_REV) which I listed on the drawing, but not for mass. It's just not there...I'm clueless!

 

[Toost]

For piece parts it's quite simple if,....
If you have a parts list., add a column which reports "$MASS" ( If you pick the Attribute names button in the Style dialog, you can select it there.)
If you like to type it yourself : <W$=@$MASS> in the "default text".

the component must have a weight calculated, the parts list will not calculate any .
RMB the component in the Assembly navigator- Properties - Weight - "Update Weight now" button.

You can set the update weight - thing as a default in the customer defaults such that NX recalculates on each Save.

The weight calculated will be the content of the "model" reference set. ( -if you have multiple solids in the same file.)
The density taken from the applied material OR, if this is not set the default density.

Reporting the weight of a component on a drawing without using a parts list is a lot of work. Using a pre-setup partslist along with the automatic weight calculation it can be automatic.

When it comes to assemblies it becomes more complex...

Regards,
Tomas

 

[Ritchie]

Thanks Tomas,

So you're saying it's easier to get the weight from a componenent when you derive it from a partslist in an assembly drawing rather then from the component itself? This means that when there is no assembly drawing (for instance a stand-alone component) you won't be able to display the weight of a component on its drawing (whereas this information is clearly visible in the part file itself)? Does it really have to be this complicated?

 

[JohnRBaker]

If you assign a material to a model and save the part, a Part Attribute will automatically be created which will be equal to to it's Mass/Weight. Then create an Expression which links this Attribute to an Expression you can then use Interpart Expressions to pass this value from the detail part file to the Master Model Drawing file where you could then create a note referencing this Expression.

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]

If you assign a material to a model and save the part, a Part Attribute will automatically be created which will be equal to to it's Mass/Weight.

Is this a new feature in NX 9? Because it doesn't happen in NX 8.5.

www.nxjournaling.com

 

[JohnRBaker]

It's been there since NX 8.0. Now it can be disabled in Customer Defaults so you might want to check to make sure that someone hasn't messed it up.

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.

 

[Ritchie]

Is this indeed a NX 8.5 feature? If so, can you be a bit more elaborate in your answer? Expressions, part attributes, interpart expressions? Can you please point out the steps I have to take...

I've been trying to figure this out for three days now, even filed an IR three days ago. Still no working template so far...

 

[cowski]

It appears that you need to have a license for the 'advanced mass properties' module for this to work as John describes...

www.nxjournaling.com

 

[JohnRBaker]

Attached is a simple part and its Master Model Drawing. You will note that there is a (excuse the pun) note showing the Weight of the part on the face of the Drawing. If you go back to the detail part file and either edit it's size or change it's Material, the note on the Master Model Drawing will update.

This part file and Drawing was created using the approach that I've previously outlined. Also note that these files were created using NX 8.0 so most of you will be abel to see exactly how this works.

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]

If you go back to the detail part file and either edit it's size or change it's Material, the note on the Master Model Drawing will update.

IIF you have an advanced assemblies license (or other module that includes the advanced mass properties). For those of us that do not have access to the license, it will NOT update, nor will the attributes be created when we create/save a part.

If, like me, you do not have the license mentioned above; I suggest you create a body measurement in the part navigator and create your own part attribute linked to the measurement expression. As the part is modified, you will need to make sure that the body measurement stays at the bottom of the list of features, otherwise edits to the model will not be accounted for. Not as nice as John's solution, but a usable workaround...

www.nxjournaling.com

 

[JohnRBaker]

One way to keep the 'Measurement' at the end of the list is to Extract a Body with the 'Fix at Current Timestamp' option toggled OFF and then create the 'Measurement' using that body. Once done, hide the extra body and make sure it has been removed from the 'Model' Reference Set.

And if you're running NX 9.0 you have an even more elegant solution to keep that extra body from interferring with downstream applications and usage. We've introduced a new 'Delete Body' function which will, for all intents and purposes, make it as if the copied body never actually existed except that the 'Measurement' feature will still update if the model is modified even if new feature are added to the model.

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.

 

[Ritchie]

Turns out I do have the Advanced Assemblies license...lucky me!

In the dummy part I have created an expression called "Mass", linked to the part attribute "MassPropMass". Why do I have to create this expression manually? It would have been so much easier and self explanatory if I could have linked the note on the drawing template directly to the "MassPropMass" part attribute.

In the drawing template I created a note linked to this part attribute: <WRef1*0@Mass>

This works, but it displays the value in grams (2711 g) as 2.711000. Units are set to grams, even in the dummy part attribute list the weight is displayed correctly...any idea what could be causing this?

 

[JohnRBaker]

If you look at my example, if I had used Mass instead of Weight, I would have had more control over the units (the method that you used provides no control as NX defaults to kilograms for the @mass function). Also my using the Note referencing an Expression, this also provides you with control over the number of decimal places.

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.

 

[Ritchie]

I'm lost, I have no idea what you are talking about anymore. So you're saying that despite having the Advanced Assembly license I still should use the work around you described earlier because when I use the attribute <WRef1*0@Mass> I have no control over the units? What is the benefit of having an Advanced Assembly license then?

Tried it the other way, using a part expression...it then says <X0.0@drf_1> in the note. At least now I can control the units and the amount of digits, true! When I turn it into a template and reference a component it just keeps displaying the value of the dummy part...

Apparantly this is so complicated that even the guys at GTAC tech support can't get it to work...it's been 3 days since I filed the IR. All I want is to display the weight of the component on its drawing, I'm not asking too much now am I?

 

[JohnRBaker]

I've already provided you with as elegant a solution as I can, and since you say that you do have the Advanced Assemblies license what is stopping you from going that route?

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.