Does anyone know how can I show the center of mass not for the whole assembly but only for one part of it in draft and if possible in assembly also.
I have an assembly of a large machine but I only want to see the center of mass for the top part of it, so in the assembly environment I create a display configuration for the top half of it, select all of it (hide everything else), go to properties and tick the "display center of mass symbol" then it shows me nicely where it is. Now when I close the properties window, then the center of mass jumps to where the center of mass for the whole machine is.
Now when I go to draft and show my display configuration for the top part of the machine and show the center of mass, then it is like in the assembly: the COM is shown for the entire machine.
I would like to see the center of mass for only my display configuration in the draft environment.
If anyone has an idea what could be the solution for this problem it would be appreciated.
I'm using Solid Edge ST6.
RMB the drawing view and edit properties, on Disply tab select part or sub assy you want to disply the CoM of and "List Coordinate Sys", select the CoM and toggle on the Show optionon the RH side of the dialog.
Note, the CoM must have been saved in the part or sub you wnat to display seperately... or it will not expose when selecting list all Coord Sys's
NOTE: the CoM symbol shown in my screen shot below is in ST9, i think the CoM Symbol was added in ST8... you indicator will be a VERY VERY VERY small point.. very hard to see so you need to know where you are looking. once you know where it is, the old advise was to do a Draw in View and draw a larger indicator or symbol connected to the COM point. you wnat to do this draw in view and connect to the point so that it stay associative...
the COM symbol only is a defined block in Your drawing.
You can change this via Options - Annotation
You also can define a different block for Coordinate Systems, to show them e.g. as axis in Your drawing
So You can have every geometry representing CS and COM to be shown in Your drawings.
The COM block came with DIN standard template in ST7 I believe
Hopefully the OP can clarify but it seems to me the poster is asking something a little different than what has been answered so far. Matt showed the COM for the whole assembly and then for one part.
I interpreted the question to be how can he display the COM for the whole assembly and then also for a defined set of multiple parts, in this case consisting of a config display group.
I suspect that's not doable without making that set a unique assembly.
There is only one CG per assembly. If I really needed that, I would make a second model with what is needed and add another view with the second CG on it. Perhaps you can insert the assembly into another assembly and use occurace properties to get it done without another copy of the files.
Thanks for the answers.
I also only see the way via an "Insert Assembly Copy" from Your original.
As said before - I think it was already menitoned - I talk about an associoative Assembly Copy rather then a copied subassembly.
So You only need to define which parts should be member of these IAC and then You show this one in Your draft
Not an associative way, but create your view config, do the mass props and make a note of the X,Y,Z co-ordinates for the measured CG and place a co-ordinate system in your assembly at that point. Call it CG 'config name' to help identify it.
You can then display the co-ord system in your drawing.
To make them easier to spot, I create a new line style called 'POINT' that is 2mm thick and coloured red.
Then set the visible and hidden edge display style for the co-ord system to POINT.
You will probably have to also set hidden edges on.