Displaying Weight Properties of Part in Drafting? 2

[mjcole]

Hi,

I'm wondering if Weight Data that can be seen in Part Properties is tied to a parameter such as Object attributes are to Parameters so PARAM=string would show up as &quot;string&quot; in drawing if <W@PARAM> was entered as text in Annotation Editor.

Is their some way to type in something similar to <&PARAM> and have that display the weight properties saved with the part.

I know you can have Assembly Weight Management shown in a spreadsheet but I can' figure out how to import this data into a Part Spreadsheet.

Please let me know if there is a way to have Weight show up in drafting so that it will update when part is changed.
If you know of any good methods or workarounds, I look forward to a response.

Thank you,
Michael

 

[cowski]

I don't have a direct answer to your question, but I do have a workaround that my company uses. We have a grip program that calculates the mass, volume, and cg point (using analyze->mass using solids). This program then sets the mass and volume to attributes; when we run the program in the drafting module it will create a note on the drawing. When the part changes, rerun the program and it will update the note. I can pass along the grip source if you think it would be helpful to you.

My company does not have the advanced assemblies licence so I don't think the weight data would even work for us.

 

[mjcole]

Thank you for your response!

The grip you mentioned would be a useful workaround that could be used with interpart expressions in drafting to work for Assemblies.

If you could send me a copy I would appreciate it. You can email me at the address shown in my profile.

I haven't worked with Grips much because I haven't learned how to do them. They can be very useful and more powerful than the Macros I use for most of my repetitive work.

Michael

 

[looslib]

We do the same thing for weight calculations. Run a GRIP program to calculate the weight, write an attribute and then display the attribute value on the face of the drawing.


&quot;Wildfires are dangerous, hard to control, and economically catastrophic.&quot;

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[bsvk]

Hi
there is away of getting this, if u don't have open grip
licence etc..
1. Name the component for which u want the mass
2. Open Spread sheet from ug modeling.
3. Create an expression called &quot;mass&quot;(or anything)
4. Extract the expressions
5. use the function in some other cell MASS3D
(MASS3D is a function which u can use in Excel sheet the syntax is:
=MASS3D(&quot;name of the component&quot;,x,y
where x is the parameter which u nee 3 for mass,
y is the units)
6. In the value field use &quot;=TEXT(cell of the mass function,&quot;no of decimals needed&quot
7. In excel give Update ug part.
8. In Drafting u can place the expression as an annotation.
If u need any more details, let me know.
Best regards,
bsvk

 

[mjcole]

bsvk,

I had a question on mass3d function and the spreadsheet.
For y value for units in the function how is this entered lb lb-in or is it a number such as 1=lb 2=kg etc. UGS sent me their descrip which says to enter y as 1 to demo the functionality.

In terms of the spread sheet when I extracted the Expressions and gave the value as function mass3d for my parameter prtmass_## = It does not update the Expressions in the model and the mass value changes to 1.

If you can clarify the above issues for me I'd appreciate that.

Michael

 

[SolidNX]

Hi Michael,

If you are using a &quot;master model&quot; structure, there is another way to get the mass on you drawings. By setting up a Parts List (defined under Assemblies), you can add $MASS as an attribute driving a field. Anytime the Parts List note is recreated, the mass will be updated. This could be forced through GRIP every time a part is say released.

Unfortunately the Parts List UI is horrible right now, but I understand it is getting an entire overhaul in NX2. Another problem is that in addition to the MASS field, you must have at least a part number (key field) and quantity field (or you could use the MASS as the key field). If you use $PART_NAME for the part number attribute though, this can be an added advantage of always showing what the file is named.

The basic steps are:
1. Define the Parts List fields in the drawing non-master. Create at least a key and quantity field and one for $MASS.
2. Turn Skip One Level off under Specify Rules.
3. Create the Parts List note.

I find it frustrating that NX cannot simply expose these system attributes ($MASS, $PART_NAME, etc.) for everyday annotation use.

Cheers,
-MikeN
P.S. Please visit

http://www.SolidNX.com

for some free utilities and other tips.

 

[SolidNX]

I was impressed with BSVK's technique, but I can't seem to get the expression to update without having to open the spreadsheet and select Tools > Update UG Part.

Combining everyone's input, I discovered that <Wcomponent_name@$MASS> will actually add the mass in an annotation. It even updates automatically after editing a component. Sometimes I've had re-opening the assembly, though. The problem I ran into was it only displays whole numbers. Anybody have any ideas how to get a few decimal places?

Example: For a component named &quot;block&quot;, key in <Wblock@$MASS>.

Cheers,
-MikeN

 

[GTI18T]

Decimal places is what I am looking for right now too. $mass works great but rounds to whole number

 

[walkersea]

As an additional question:

The results from an Analysis.. Measure bodies.. then either of the four options - volume, surface area, mass, radius of gyration - these values can't be used as attributes either referenced by the drawing or in other expressions?

I can't GRIP - and to be honest I'd rather not have to. I do need to be able to define material attributes for a part, and then have the part calculate the mass based on the geometry and report it on the drawing. It would also be nice to be able to use the attributes to allow an expression for displacement to be an attribute of the part as well.

We do not have the advanced assembly modeling module - so no weight management. Should I be looking at getting it?

Regards.

 

[Vikingbro]

walkersea,

Could you clarify your question concerning the 'Measure Bodies' issues?

I can perform the 'Measure Bodies' function, saving the results. From there, I can access the expressions in Drafting - at least when creating a note.

Go into the 'Annotation Editor', then click the ' Annotation Editor' icon, then click the 'Relationships' tab at the bottom of the window. From there, click the 'Expression' icon. You will then get the expression list. Scroll down the expression list to the desired expression. When you click on the expression, you will get something that looks like this:
"<X0.2@p14>"

The number following the decimal point is the number of places that will be shown in the note.

Play around with it to see if you can get it to work for you.

Good Luck!

Chris Cooper
Cleveland Golf / Never Compromise

http://www.clevelandgolf.com

http://www.nevercompromise.com

 

[MSPBenson]

Major downside to the 'Measure Bodies' technique is that you have to remeber to move it so it's the last feature in your tree.
If UG change it to have no timestamp it will be the ideal tool.
Does slow down model updates too.

Mark Benson
CAD Support Engineer

 

[jackley]

You could always just save all the information from 'Measure Bodies' to expressions and then rename the ones you want to keep it simple (p458 is volume, rename it to 'volume')

Then in your notes, do as Vikingbro said, <x0.2@volume>.

Now, does this automatically update when you go into your drawing format? Anyone have any input on this?

 

[jackley]

I just checked and it does update when going back into the drawing format (for those that don't know).

 

[walkersea]

OK - I see how this works in a part. If the save option always set the expression parameter to the same value it wouldn't be too bad, but as it changes dependent on the model, then we will have to manually assign the correct name to the parameter required for every model created - this is tedious!

I'll have to experiment - it could be we have basic parts (e.g. cylinder shape, block shape, etc) that already have the expressions in - will these then update correctly as additional features are added?

Do you use the Assign Material.. to set the material properties (particularly density), or is this just available if you have Strength Wizard?

As for the assembly - how do you get the total mass of the assembly?