Copy Geometry or some other method

[NathanMantz]

I'm looking for some advice on methods of showing "reference geometry" in an assembly - specifically a drawing.

It looks like copy or publish geometry is correct, but the selection set rule is greyed out and I cannot select "entire" parts of the assembly I want to reference.

I'd appreciate any suggestions.

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[RickGiguere]

HI

If you just want to show certain 'parts' of an assembly in a drawing, you can create a simplified rep of the assembly with the parts you want showing; save the view, (may need to save the model too), then create a drawing of the assembly; in view proprieties pick view state, find simplified rep and scroll to the view you saved in assembly mode.

I don't know if that is your question, but that's what I thought you were asking.

Rick

[NathanMantz]

Thanks Rick,

I guess I should have added more detail to my question. Your suggestion is what I have done, but the mass properties calculates for the "entire" assembly, and I only need it for a certain portion.

I have a family table of a weldment that needs a drawing of installation instructions. Sheet 1 is for instance 1, sheet 2 is for instance 2. The drawing title block displays the parameters assigned to the generic, and I need to reference 2 other, parallel-level components for the locating dimensions. One component is a part, and I was able to select the surface when defining a copy geometry feature. The second component is an assembly of 80-100 parts, and I am unable to select the assembly when defining a second copy geometry feature - so far, I have only been able to select one part of the assembly.

In my drawing, I need to reference the 2 other components, and have them show as "reference" for dimensioning, yet not appear as part of the BOM, and need those 2 components not affect the mass properties calculation, but I also don't want to spend the rest of the day defining each component as individual copy geometry features. I also tried working with publish geometry with the same result of not being able to select the "entire" assembly that I wish to display.

By creating a simplified rep of the main assembly, I was able to insert drawing views and models in such a way that the BOM displays only the weldment assembly which I need, but then I used view|drawing display|component display to modify the geometry I want to reference into phantom line display. As I'm typing this, I'm wondering if my issue would be best solved by figuring out how to have the title block reference the simplified rep for the mass properties - is it possible?

For example, sheet 1 of my drawing has &PRO_MP_MASS:29[.1] in the table cell properties, and the mass of the entire assembly is displayed. Sheet 2 &PRO_MP_MASS:39[.1] and the mass of the simplified rep is displayed. Where or how do I figure out where this nomenclature comes from, and which is the correct string to input for sheet 1.

n

[RickGiguere]

Hi

I have no experience at all at what you are trying to do, but try switching the 29 and 39 ID numbers and see if the mass properties change in drawing 1

When I take a part(s) off an assembly using a simplified rep, the mass changes.

Have fun, I've never tried anything like this.

Rick

(edit)

I edited my post, took some erroneous wrong info out.

If I open an assembly and check the session ID for the master rep, and then open a simplified rep of the model and check the session ID #, it's the same as the master rep. I have no idea where those 29 and 39 numbers are coming from.

[.1] may be the session ID #, they're both the same

[Kevin]

Not knowing exactly how the drawing and its assemblies are set up it may be those are the session ID's for the main assembly and a sub assembly that just happens to have the components that are required (which may be another way of getting what you need). The [.1] controls the number of decimal places.

[NathanMantz]

Kevin, thanks for the session info tip - now I understand which witch is which.

I've given up for the day - can you tell me if there's a way to print or view all session info information for a given assembly?

[Kevin]

I don't think there is a way to show all the session ID's at once. If the models are added to the drawing when you type in the note for the mass ProE will attach the session ID for the active drawing model. So all you would need to do is set the model you want the mass for and type &PRO_MP_MASS or &user defined parameter name.

[Kevin]

One thing you can try that may work is create an external simplified rep and add it as a model to the drawing. To determine the session ID (number after the colon) select tools>relations>show session ID with the main assembly selected. In the menu manager you can select Assembly and Name to get model info and select the external simplified rep to get the session ID.

[RickGiguere]

If an external rep was created minus these two components that will be used for references, it 'may' create a session ID #, and calculate the mass minus these two components. Then you could use this session ID # in the master rep, which will show all the components, but have a mass minus two components.

I don't know if external reps create session ID #'s, the one I created didn't have one, when I checked it was grayed out.

I guess it would be good to know what creates a session ID, I don't know.

I was looking at what sequence components are brought into an assembly, really didn't tell me much.

Parts don't have a session ID, if you open a part and check for a session ID there isn't one.

Rick

[Kevin]

Parts get session ID's in assembly mode. They also get session ID's if you have more than one part model added to a drawing. Parts are assigned even numbers and assemblies are assigned odd numbers.

[DavidButz]

Nathan,

I'm not sure I totally understand your problem, but I hope you are not making things unnecessarily complicated for yourself. It sounds as if you actually have two issues: (1) Having appropriate "outside" reference geometry available in the drawing, and (2) accessing the correctly referenced mass properties. Is that the case? One suggestion in regards to #1. You mention that you can get the Part reference using Copy Geometry, but not the references from a Sub-assembly. You might try creating new Surface features within the top-level assembly by copying the necessary reference geometry OR by creating appropriate Datum features with respect to that geometry, then select these Surface and/or Datum features for copying. I don't know if that will help you or not. As far as the mass properties are concerned, if you can produce the desired results with the "&..." method, you should be able to place this as a Note or within a Table without reference to a particular view or sheet. Good luck!

David

[NathanMantz]

Thanks to everyone for their help.

Nice to learn about the session ID - not sure where I would have found out about that otherwise.

Based on everyone help, I've created a Geometry simplified rep, and a "simple" simplified rep. The second simplified rep excludes the geometry that I wish to refer to.

I placed views of my top assembly as the Geometry Rep, and used View->Drawing Display->Component Display to change the view properties of the assembly that I wish to "refer" to.

Then I changed models to choose the second simplified rep, showed my subassembly in exploded view, and replaced the page format to generate a new BOM table.

I was able to display the BOM table with only the components of my subassembly, and not the components of the other assembly which is what I want.

I was not able to place dimensions from my subassembly to the top assembly, as limited by the Geometry Rep, I think I could have used the master rep instead, but that's what I was doing when I started this discussion.

I also used the session ID for sheet 1 and sheet 2 to display the different mass properties of my 2 instances.

I will have a look into the external reference rep to see how I could use that, and I think I will start a new thread to learn how ProE chooses precedence of models to use for a title block.

Nathan