There is a family of tubes that are cut to a raw length. Then they are run through a press to add a stamped hole and a piercing that gets tapped. Currently the family is built around the second step in that the the main diameter of the tube is extruded and the the piercing and hole are added (negating the fact that they come from a pre-cut tube length).
I was going to brake these appart so that the BOM called a tube in an assembly and then I was going to add the piercing. I forgot one thing. You cannot add an extrude in an assembly (only a cut/extrude). Any thoughts or suggestions on how to procede?
Why is it that the Pink Floyd's song The Wall comes to mind every time someone wants to do something only to get whacked with a ruler across the knuckles by the "teacher".
It is so odd that PTC doesn't recognize the need to "re-strike"... a form operation that happens at a next level assembly. This is so common in the industry!
I have seen a tutorial on a progressive die tutorial from PTC. They make extensive use of merged features from one level to the next. I cannot wrap my head around the logic, but there it is.
Let us know what you come up with.
As for now, I will live to fight another day. Now I know why they didn't do that. We'll have a dumb BOM at that level for now and just keep it that way.
I let you know if I come across something else and can go from there.
Do you or any of your collegues have a suggestion about a way to add materail in an assembly (move material in this case)? If I form a tube by punching it with a press and get the boss on the inside while referencing it from a blank tube in an assembly.
You can create the feature at the part level in the assembly and then suppress it at the part level. To show it at the assembly either create an explicit family table for the tube with the feature resumed or use feature flexibility to resume the feature at the assembly level. This method creates an external reference from the assembly to the part, but as long as PTC won't allow material additions anywhere except parts there isn't an easier method.
If you are using the same tube in a lot of places and don't want to end up with an endless feature tree, create separate parts that inherit the base tube and use those in the next assembly to capture the added features.
Currently it is suppressed in the basic cut tube and then unsuppressed at the "next" level. It is just that the BOM is a typed in BOM instead of calling the blank tube paramters (since they are the same paramaters used in the pierced tube - which are then used in the next level up).
"Currently it is suppressed in the basic cut tube and then unsuppressed at the "next" level. It is just that the BOM is a typed in BOM instead of calling the blank tube paramters (since they are the same paramaters used in the pierced tube - which are then used in the next level up)."
If this is a question or a problem to be resolved, how are you unsuppressing the features at the next level?
If you are just saying that you already do what I suggested to manage the features, then OK.
Currently adding material (or any feature) to parts in assembly context only is not supported.
Assembly-specifc context variations are available either as:
- Remove material - by assemly cut
- Change dimentions and parameters - by flexbile components/features
For the challange you are describing - there are two options you may consider:
1. If you wish to use *same* object for the different steps of the process (before/after adding the features) in different drawings - you can use part simprep and suppress the features as needed per drawing.
2. If you wish to have different object per step in the process - you can use Family-Table or Inhgeritance features.
We will consider in future releases to support part-level features addition in assembly context (similar to flexible components).
Hope that helps.
We currently have a family table and the features are suppressed in the blank tubes. The parameter for part number calls out the tube in the tube part and the peirced and tapped tube in its part.
What I was hoping to do was create an assembly that is the blank tube. After it is pierced and tapped, it becomes another part. So when creating a bill of material for the pierced and tapped part, I was hoping to have the pn in the BOM be the blank tube, and after words be a new number.
i.e. the blank tube is P/N 1234, the pierce and tapped is P/N 1235. I have a parameter in the family table for the part number (P/N), but if you call the part number in the pierced and tapped part, it will call it's own and not that of the blank tube.