I'll try and explain this the best I can.
I have assemblies that are comprised of reference parts - the assembly is a purchased part such as an air cylinder. I have them as reference only in the assembly (ie right click on the parts in the model tree->BOM Reference->Reference). I do it this way so I can adjust the air cylinder how I need it, but still only asign one part number to the whole assembly - as an example we'll say "cylinderX" is the part number, and filename is "cylinderX.iam"
The problem arises when I put cylinderX.iam into other assemblies and try and make drawings of those assemblies. Even though cylinderX.iam is not a reference part (but all it's sub components are), it shows up in an IDW just like reference parts. I am able to make it show up how I want by editing the view properties (Edit View->Model State Tab->Reference Data Line Style "as parts"), but I still cannot balloon cylinderX.iam. It shows up in the parts list, but I cannot attach a balloon to it.
Solved! Go to Solution.
Hi! Purely based on the description and my past experience in this area, it sounds like either a corruption issue or BOM View is not set properly. Could you show me an example of this behavior so I can take a look closer?
If I might suggest that instead of making your air cylinder parts (ram,body,seals etc.) reference, you set their part BOM structure to phantom.
If you never make or purchase the individual cylinder parts then as far as your BOM is concerned they do not exist.
The only part that exists is the purchased cylinder assembly complete.
Inventor is seeing all the edges as reference and so ignores the complete assembly as far as ballooning is concerned, it's as if you have placed an empty assembly.
The assembly has BOM structure but no physical body.
Rather than "(ie right click on the parts in the model tree->BOM Reference->Reference)" in the assembly, edit each of the component parts of the air cylinder.
Use the following procedure to change the default BOM Structure setting for a part:
1.Open the part.
2.Click Tools tab>Options panel>Document Settings to display the Document Settings dialog box.
3.On the Bill of Materials tab, set the Default BOM Structure value. (Phantom).
This should make your assembly essentially a part, show the correct line detail in drawings and allow ballooning.
Hope this helps.
You have discovered the one bad thing about references. If an assembly is set as reference in one assembly, it will show as a reference in every assembly. You can set it to a purchased part if you want to baloon it.
If you then want to exclude it from the BOM on purchased, just use the filter.
If you want to make it look like a reference part, simply open the view in the drawing browser tree, find the assembly, right-click it, select properties, and change the linetype to whatever style you like and the color to grey, etc.
This solved my problem, thank you!! I've only ever used phantom for subassembled items that I only wanted the components to show up in my BOM and not the subassembly (ie an assembly of a bolt, washer, and nut). So this is like the opposite of that.
The only issue is that in rare instances, one of the parts in the subassembly is a part that we purchase (or make) separately. I worked around that with a dummy partno/filename for the phantom part.