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Insert partdimensions in bom's

pep

New member
Hi,



Some parts and assemblies are driven by relations. Now I wanna make a bom (table), but one colom can't be filled in because of variable dimensions. Is there a function for this problem ? And do I have to use it ?



Kind regards

pep
 

mmead0ws

New member
Could you clarify a little? How do the relations drive the assembly? How does this relate to the column that can't be filled in?
 

pep

New member
Hi,



some parts of the assembly are related to each other, eg d0:32=length:74-2*d0:56+50. Length:74 can be set by a layout, so the designer is able to fill in this dimension. When length:74 has been changed, d0:32 will be adapted. I want to put a bom to the drawings, but the value of this variable parts is unknown beforehand. Is there a function, eg &asm.mbr.prt, to solve this problem ?
 

mmead0ws

New member
Assign the value of d0:32 to a parameter first (parameter = d0:32). That will give you easy access to its value in the report table. I'm not sure which report symbol shows this parameter in the table. It is probably mbr... or mdl...



There may be two options for representing your flexible assembly in a drawing(s). If your design has a range of values (i.e. 1.00-100.00) you can use the parameter representing d0:32 in your repeat region directly. The value of that parameter will change each time you change the configuration and regenerate. So you will have a different released drawing for each released configuration. It isn't a problem for engineering to create because the Pro/E drawing updates automatically.



Some companies use tabulated drawings so they only create one drawing for all configurations. It would take a family table of the variable component(s) to do this. If the driven component has a finite number of configurations, it can become a family table. Using a family table, you can create a new table on the drawing listing all instances and their dimensional differences. From the original table, you can write report table relations to show See Table when the specified component is encountered.



Can I make a suggestion? Please don't use session IDs :32. Session IDs change every time you restart Pro/ENGINEER or every time you clear the assembly from memory and reload it. Instead use component IDs. These numbers never change. Just add a column to your model tree for component ID. In parts it is called feature ID. Use it like this:



d0:CID_## where ## is the component ID

d0:FID_## where ## is the feature ID



Wildfire allows you to use the name of the feature or component instead of the ID number. So it becomes d0:CID_<component name>.



Hope this makes sense.
 

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