Modeling Heli-Coil's within a large assembly

[kacar]

I wanted to get some opinions from other users on the either the best way to model Heli-Coil's within assemblies or at the very least how they model Heli-Coil's within their assemblies and any issues that you may have encountered. I have heard of 3 methods of doing this:

1) Not including Heli-Coil's at all in the assembly as they slow down the assembly considerably

2) Creating a solid model of the Heli-Coil part. 

3) Creating Heli-Coil's as a surface

[GaryLinscheid]

We model ours as a hollow cylinder solid model.

[TomD.inPDX]

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.

[Dale_Rosema]

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

[Dale_Rosema]

Forgot to mention that the nice with the dummy model is that all of the parts that are of this ilk are located in the same file. I just waste a little time when it opens as I wait for the model to refresh on the screen and then  I realize that there is no model to refresh on the screen.  

[TomD.inPDX]

I've used dummy parts before to account for the BOM.

I like the idea of grouping them in a single assembly file.

[Dale_Rosema]

Could have been you from which I learnt this practice about 5-6 years ago?

[TomD.inPDX]

🙂  I've probably forgotten more about Pro|E than some people will ever learn.

[KenFarley]

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.

[dgschaefer]

I thought about suggesting a bulk part earlier, but the in many cases a bulk item is used "as required" and BOM relations are created to list them "A/R" or somethign similar.  If you create things like Helicoils as bulk items, they need an exact count but your BOM relations will tag them "A/R".

Using the "Dummy" part idea, you can assemble them to the hole locations and if the holes are patterned, the qty will update as the pattern changes.

[TomD.inPDX]

I like that a lot as a standard for managing A/R items.

First of all it could carry a valid assembly part number (per your organization, of course)...

And you know that only items that cannot otherwise be accounted for are here.

In this way, Doug, are you saying you got BOMs to regenerate without edits between document revisions?

Not sure I'd throw helicoils into an A/R bucket though.

In my industry, inseparable hardware is not an accounting item.  It is part of a purchased part.

I will model the PEM hardware and assemble an .ASM for a full 3D representation of the as-purchased part.

This also means that every full BOM (default PTC versions) will break this down to the PEM.  And I want BOMs to stop at the "purchase" level.  See how these little details in how to manage a model can have implications?

<rhetorical> Point being that having a well thought out plan at all levels requires much consideration.  I've also been trapped in so many ways that the creative process is stifled by control.  Today I manage 3 wholly different processes in real time.  Simplicity is the watchword at every level.  Covering all your basis makes things simple.

[dgschaefer]

---

@TomD.inPDX wrote:

I like that a lot as a standard for managing A/R items.

First of all it could carry a valid assembly part number (per your organization, of course)...

And you know that only items that cannot otherwise be accounted for are here.

In this way, Doug, are you saying you got BOMs to regenerate without edits between document revisions? 

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Tom, I'm not sure what you are asking, can you clarify?

I was arguing against using a bulk item for helicoils as well.  We, like a number of companies, use repeat region relations like this to change the qty of bulk items to A/R:

IF asm_mbr_type == "BULK ITEM"
quantity = "AR"
ELSE
quantity = rpt_qty
ENDIF

Unless you don't care about specifying the quantity of helicoils, then using a bulk item would break this functionality.

The suggestion I was making was to use the dummy (solid) part method mentioned above but instead of assembling them by default, create just enough geometry (a CS at each hole perhaps) to tie them to the holes they go in.  That way, assuming that your holes are patterned, as the hole qty changes, your number of helicoils will update too.  That said, having some geometry in the helicoil would give a visual confirmation that every helicoil has been placed.

[KenFarley]

I definitely agree that putting some sort of model in the assembly takes a possible source of error out of the process. I also prefer to have actual geometry so when you make section cuts or exploded views it is obvious what is to be done, and you will also have a visual verification that you're using the right length insert, pem nut, or any other multi-versioned bit of hardware.

[TomD.inPDX]

@doug...  I was asking if you have found a way to incorporate every possible (reasonable) event in Creo modeled assembly structure that accounts for an acceptable BOM without manual manipulation of said BOM.

[dgschaefer]

---

@TomD.inPDX wrote:

@doug...  I was asking if you have found a way to incorporate every possible (reasonable) event in Creo modeled assembly structure that accounts for an acceptable BOM without manual manipulation of said BOM.

---

In a word, no.  We frankly don't do a lot of assy documentation, but I have a way to accommodate bulk items as A/R and to replace the index number with N/S for items that are included and not shown on the drawing.  That's all I've worked through at this point, and frankly I haven't even worked them into our default templates yet.  I apply them as needed.

[TomD.inPDX]

I was hoping 🙂  This is one thing about Creo if you don't have Windchill.

There is a lot to be said for not trying to manage BOMs within core-Creo.

Having said that, I make BOMs from scratch. 

A little more work but a whole lot more control.