Modeling Heli-Coil's within a large assembly

We model ours as a hollow cylinder solid model.

If you had a 1,000 inserts in an assembly that was built into the next 5 levels of assembly and drawings, you need a strategy.  And you have options.

Most likely you will need something in your fabrication drawing.  You probably have a section somewhere that the heli-coil is visible in section.  You have to account for this.  Sketching one on a drawing sucks to say the least.

Manage your next level assemblies:  You can use family tables or even display states to manage what is used at the next level.  This means you can lower the graphics load by ignoring these miniscule features at higher level assemblies.

A "symbolic" thread representation is a surface in Creo by default (cosmetic thread).  They are worthwhile in a model but often get in the way on drawings.  You can turn them off quickly in drawings by editing the view (RMB(view)-hide cosmetics (?)).  This could make for a lot of little surfaces.. one for the heli-install thread in the part and two in the heli-coil model.  Seems like a lot of effort.  In most cases, the most you would need is the mating thread to another part in the assembly.

How do you manage other press-type fasteners?  Heli-coils are no different than a PEM feature for instance.  How do you manage those?

For me, I would model the heli-coil as a solid; add the appropriate chamfers to mimic the major thread diameter; leave the major diameter of the heli-coil the actual size and without a cosmetic thread; and the insert hole in the part as the tap-drill size with no cosmetic thread.  In a drawing, you can probably change the linestyle of the interference to dashed for a proper thread representation.  Otherwise you can sketch the line.  This should be a very limited operation only to satisfy the drawing.

I have not run into the situation where the overall size of my file was too big.  But I would manage file size issues with one of the many means Creo provides in keeping data manageable.

For things that need to be in the BOM and don't really need a model, I have created something I call dummy models.

Dummy.prt

In the dummy model, I have a family table. The family table consist of the columns of information that will show up in the BOM. If I need 6 polybags in my packaging, I assembly one polybag of a particular size at the origin of the packaging assembly and then pattern it 6x at a distance of .001" vertical from the origin. The BOM will then call out 6 polybags of that particular model.

Thanks, Dale

There is another option, but it provides no visual representation in any of the drawings. You can make a bulk part (File->New with type "Part" and Sub-type "Bulk"). It's an empty part that just has parameters. You will need to add the parameters that are used in your bill of materials tables. You set the BOM_report_quantity to the number of the helicoil you need in your assembly, and it will show up in the Bill of Materials. The bulk model will have a family table, so you could do something like name it "bulk-helicoils" and add entries for each type/quantity you require.

We use this a lot for things like adhesives or threadlockers, rubber strips, etc.

The bad part about this is that the quantities are not parametrically defined by the geometry in the parts, so if we add some holes we have to remember to change the report quantity manually, which can bring some errors into the process.