Ok ... now that the weight data for all the components is available in the assembly is there a way to sum the weights of them and use that for the weight of the assembly?
The reason I am asking is because now I am getting the weight of the assembly by putting a "body measurement" feature in there and getting it from the expression - but if there is a way to bypass that it would be nice.
Left hand may not be speaking to the right hand!
You would need to do the assembly analysis and assign the result to an attribute to put it on a drawing.
That's how we used to do it. Unless NX can capture the values automatically in attributes.
When threaded holes first came out in V14, all the data was in the model, but the drafting side had no way to use that data in a drawing.
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Ben is basically correct; create a Measurement Expression for weight at the Assembly level and reference that Expression value in you Drafting note. However, I must caution you that the Measurement Expression is not quite as 'smart' as it really needs to be in a situation like this. Now, it has no problem updating if and when any of the Components change in size (and thus weight) or a different material is assigned (also changing the weight of the Component), but it will NOT update if additional Components are added to the assembly at a later date since the Expression feature ONLY remembers the bodies of the Components loaded at the time the Measurement Expression was created. So if the number of Components do not change, only their size/shape/material, this works fine. However, if you do change the number of components, you will need to recreate the Measurement Expression and make sure that the Drafting note is now referencing the new calculated weight value of the updated Assembly.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
I think it has been mentioned before, but for the sake of having the information and letting you decide what to do with it, I prefer to create the measurement expression used for weight expressions at the drawing level. I guess this is just because I tend to differentiate between the task of maintaining the model and the task of maintaining the drawing differently in terms of our work-flow and releasing cycle. You'll also find that this expression changes and will ordinarily need to update itself every time the model changes. I find that I'm regularly working in the context of my assemblies even while I don't generally have the drawings open so while I'm changing the model there's one less feature update to worry about and wait for.
OK, now I have all the materials assigned in my assembly, and the weights are displayed in the Assembly Navigator and the total rolls up to the top level. Now, my ultimate goal is to determine the CG of the assembly. So far I have used Analysis --> Measure Bodies and simply selected the entire assembly by windowing around it, but I can't be certain all of the components are selected. Is there a better way?
If you go into Analysis>Measure Bodies then you tick associative on, then it will create a body measurement feature, five expressions and a point at the COG. My understanding is that it requires solid bodies to measure rather than components and these are usually filtered for by default. Fitting the model to your screen and hitting the select all icon are about the best way to ensure that you don't miss any.
Is there a way to assign a material or density at the assembly level? I'm working on a drawing (master model) where the model did not have a material assigned (the part is not made of the default steel). I have tried 'assign material' and 'edit solid density' but neither command will allow me to pick anything.
One of the models does need to be changed; for that one the obvious answer is to assign a material before I save the file. There is another file that I will not have access to, any help on that one?
Technically, I can get access to the file but it requires some paperwork. As we create drawings, I have a feeling that we are going to find a dozen or so files that need a material assigned. I prefer to avoid all that paperwork if possible.
OK, here's a workaround which you might want to consider. Create a new empty Component in your Assembly, set it to be the work part and then WAVE link a copy of the solid body from the part file which you don't have access to. Now delete the original Component from your Assembly and open the new Component as the displayed part and assign your material to the body that you find there (you may also want to copy all of the Part Attributes from the original part file to this one as well). Go back to your assembly and save it. Now you should be able to see the correct information in the Assembly Navigator. Of course you may need to play with the name of the new component so that you know what it's heritage is, but since it's still linked to the original model, any changes made there can be migrated to the new part file thus keeping your assembly and weight information up-to-date.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
