Drafting Mass, Inertia, CG automatically

[ingallspw]

Does anyone know of a way to automatically calculate the Mass, Inertia, and a Center of Gravity and add a call-out onto an assembly print that automatically updates each time the part is changed?

On a side note...

Is there a true way to draft the center of gravity? I've only seen it on one other print and I doubt the method I saw is a part of any ANSI spec (or equivalent).

Thanks

Keegan

 

[JohnRBaker]

I assume that you're talking 'Moments of Inertia', correct?

Well Mass and Center of Gravity can be done, with a little work, but Moments of Inertia will be a bit trickier.

But first, what version of NX are you running?

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

http://www.siemens.com/plm

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

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

 

[ewh]

Keegan mentions NX6 in another thread.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[ingallspw]

I use NX6.

Thanks!

 

[ingallspw]

NX6

And yes, Moments of Inertia.

Thanks,

Keegan

 

[SDETERS]

With the center of gravity do you have to give each part its own material from the density point of view? Going to watch this thread Wondering how this is done in NX6. Good thread

 

[ewh]

Yes. I'm sure that John will be better able to explain than I would.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[hudson888]

I'd imagine that you could create a macro to do what you need. I don't know how you'd show the moments of inertia on a drawing exactly, but some of the other stuff is readily set up to work with expressions and the centre of gravity can be saved as a co-ordinate system. In later versions setting up an associative measurement under Analysis>Measure Bodies will create a point at the COG and maintain expressions for volume, area, mass, weight and radius of gyration. Any of these can be displayed on drawings using relational annotations.

The good news is that these expressions are automatically updated every time the part is changed.


The bad news is that these expressions are automatically updated every time the part is changed.

Because it takes some time. However the measurement is just a modelling feature that can be suppressed until you need it just as long as your mindful of how you're managing the process you'll be fine. I operate that way all of the time.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

OK, here's an example of a Drawing where I've got a note reporting the Weight of the Master Part as well as the Center of Mass (shown as a point in the drawing). Note that any edit the Master Part model will be reflected in an updated drawing (if the update doesn't occur immediately, perform a Tools -> Update -> Update for External Change from the Modeling Module). Now if you are simply editing the model, there is not much else that you have to do, but if you add any additional features, you will need to go into the Part Navigator and reorder the Measure Body feature to once again be the last feature in Timestamp Order. Also, if you edit the Material assignment this will also update the Mass values.

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

http://www.siemens.com/plm

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

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

 

[ingallspw]

Awesome! It can be done! Could you break down how you made that model? I get the P33 expression but I am not sure how you knew it was P33. I also do not understand how you made the center of gravity point.

I'm thrilled it can be done though!!!

Thanks,

Keegan

Oh and also I found a COG symbol:

http://www.virginiadot.org/business/resources/Cells-Symbols.pdf

Page 2, second line down

 

[JohnRBaker]

The p33 expression was whatever was assigned to the Mass when you created the 'Measure Body' feature, which can be done either inside the Expression dialog using the 'Measure Bodies' option at the bottom of the dialog, next to the f(x) option, or you can use the Analysis -> Measure Bodies... with the Associate option toggled ON and you will get the same Measurement expressions.

As for the 'smart' COG point, that's created automatically when you create the 'Measure Body' feature (in fact, the 'Point' IS the feature), but to make sure it gets included in your drawing, you will have to manually add the Point object to the 'Model' Reference Set.

What I've done is added the required Expressions and Attributes to my default Part Templates so that if I ever need an Attribute, for whatever reason, which tracks the mass/weight of a model, most of the hard work has already been done. All I have to do is create the Measure Body feature and edit one Expression linking it to whatever p-number was assigned to the Mass/Weight value of the model. Note that depending on whether you're working with Metric or Imperial models, you will need to do things slightly different if you wish to get the normally used values for what we generally consider as being the 'weight' of an object. In Metric parts, you use the value for 'Mass', whereas with Imperial parts (AKA English units), you use the value for 'Weight'.

To help you out, I've attached copies of both my Metric and Imperial default parts with the predefined items already in place. All that I do is build my model and when I it's complete I create the Measure Body feature, go into the Expression system and edit the expression 'Mass' ('Weight' in an Imperial part) setting it equal to whatever p-number was assigned to the value for 'Mass' ('Weight' for an Imperial part) measurement expression.

As for the Drawing, once you've created your drawing, create a note where you set the value equal to an 'Object Attribute' (using the 'Relationships' option) and then select the Component in your Master Model Drawing (while in drafting, you will need to use the Assembly Navigator to actually select the Component) and select the 'Weight' attribute.

Attached are copies of my two Part Templates (they are in NX 5 format). You may also wish to look a the other default attributes which I include as well as the default display setup and so on.

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

http://www.siemens.com/plm

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

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

 

[hudson888]

John,

I check out you model and I do much the same thing except that I take the measurement at the drawing level. I suppose its much of a muchness either way, but I wondered what anyone thought of the relative merits of doing it either way.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[ingallspw]

So far what you have shown is gold! So to pry any further I feel like I am taking advantage...

I've gotten the COG drafted and automatically updating and I've also added the weight as a text field in the title block. Now I am down to adding the Inertia.

I would need to use either the calculations from the "Moments of Inertia (WCS or Centroidal)" These are the results I am getting and the output that I want to appear on the print.

Moments of Inertia (WCS)
Ix, Iy, Iz = 346.14661714892, 677.16928209864, 345.37266325727

Moments of Inertia (Centroidal)
Ixc, Iyc, Izc = 345.80884898495, 677.16927178071, 345.03490541115


INERTIA 677.16927178071/(32.174*12) = 1.75392468 lb-in-sec-2


And Hudson, as far as drafting the inertia, I just want it to appear as a text field in the title block.


Thank you to all of you so far and this website!

Keegan

 

[ingallspw]

Hudson,
For me (or the company I work for), I think it makes more since to put it in the drawing file as well. I say this because once all that info is in the drawing I shouldn't have to go back to the model to get those calculations.

It also makes it easier to modify the model without having to wait on the Mass properties to update. Once the modifications to the model have been made and finalized I can then update the drawing and mass props.

I'm a bit scatter brained at the moment so hopefully that makes since!

Thanks again to all of you!

Keegan

 

[hudson888]

As John says he does it using a template and that makes some sense but I work the way that I do for the very reason that you stated.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[potrero]

John,
Can you comment on how to apply the Associative "Measure Bodies" approach for assigning a MASS parameter to parts, to Machinery Library parts?

For example, if I have an assembly containing a bunch of Machinery Library screws, how do I obtain their masses? What if one wants to use a custom material for the Machinery Library parts (and thus a different weight than default steel)?

In general, how does one handle this issue with Family parts?

Thanks.

 

[JohnRBaker]

You would have to assign a Measurement feature to each of the Part Family Template files as well as the expressions to drive the attributes, which would then be inherited by the each family member as they were created. If these were done using consistent names then they could in turn be linked to the upper level assembly and utilized however you wish to do so.

That being said, if your goal was simply the overall weight of an assembly, including all of the component parts (would include the standard or purchased parts, such as fasteners from the Machinery Library), you could create the Measurement feature at the assembly level (including a Master Model Drawing) and simply select ALL of the components. Now this will result in a single value for the entire assembly. Now if changes where made to the master parts such as changing the size or the material assignment, this would automatically be reflected in the Measurement expressions at the assembly level as long as the original components were still part of the assembly (even if they've been modified). Now if new parts were added or existing components removed/replaced, then the Measurement feature would have to be recreated as we do not yet have a automatic mechanism which would 'recollect' (reselect) the components to capture any new/replaced/removed components whenever there were any changes made to an assembly.

Anyway, you can get a fairly good arrangement in place with the current tools, which can handle the normal updates, with just a little extra manual intervention needed for a few of the more exceptional situations.

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

http://www.siemens.com/plm

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

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

 

[ingallspw]

That's a good question Potrero! And thanks John, I've never thought of doing things that way!

 

[ingallspw]

Am I doing something wrong?

I have a fairly large assembly and if I Measure the bodies and select "Associative" it gives me the results I want (except inertia) in about a minute after selecting the bodies.

(yes there is always a big but)

But... when I click OK, it sits there for about 15 - 20 minutes. I don't get it because before hitting OK, the results are displayed and, I'd think, should already be stored and calculated, so why the huge delay just to create a few expressions?

Any suggestions ju all?

Thanks!!

Keegan

 

[potrero]

@ingallspw, I've definitely noticed what you're describing but unfortunately can't give an answer as to why it behaves in that manner. Someone else?