Not a Reference Part

[dan_inv09]

2008

Detailed explanation: coupling with a set screw, I had the two halves and the insert in one assembly but I would prefer not to have a different part number for each possible combination of hub sizes (and fits etc.) but now the screws that are not purchased separately are in my bill, so I tried making them reference.

Simple question: How do I keep something out of my bill without it bleeding through everything in a heavy dotted line.

[DewayneH]

Try changing the assembly BOM structure of the coupling and set screw to purchased.

[Inv_kaos]

You could filter your parts list to use your ViewRep, but this will not keep it out of your BOM. The easiest way is to use a reference part in BOM and change the style used in the .idw for reference parts or only the reference parts of interest.

Regards,
Stew

[Anonymous]

Edit your drawing view and on the Model State tab, set Reference Data Line
Style to "As Parts", and you'll also likely want to change the Hidden Line
Calculation to All Bodies.

Hope that helps,

--
Andrew Faix
Product Design Lead
Autodesk Inventor

wrote in message news:5990252@discussion.autodesk.com...
2008

Detailed explanation: coupling with a set screw, I had the two halves and
the insert in one assembly but I would prefer not to have a different part
number for each possible combination of hub sizes (and fits etc.) but now
the screws that are not purchased separately are in my bill, so I tried
making them reference.

Simple question: How do I keep something out of my bill without it bleeding
through everything in a heavy dotted line.

[dan_inv09]

That's what I needed.

Thanks everyone, but this was one of those cases where I just didn't know how to use the functionality. It was there all along and I just never knew what that whole part of the edit view dialog was for.

[Anonymous]

Put all the coupling parts in one assembly and set the assembly "default BOM
structure" to "phantom". Also change the set screw "default BOM structure" to
"phantom".

When you place this coupling assembly into another assembly, the BOM will only
show the coupling halves and the insert. The "phantom" assembly and the
"phantom" set screws will not show on the BOM. Visually, on the drawing, they
will appear as normal parts with normal object and hidden lines.

You will have to make the "phantom" BOM change in the IPT file for the set screw
itself as this is not an option at the assembly level. I would put this
particular set screw IPT file in the same directory location as the coupling
parts and keep a separate set screw IPT file with its BOM structure set to
"normal" for instances that you DO want the BOM to show.

Phantom parts (like your set screws) are actually used in an assembly but do not
show on the BOM. Reference parts are NOT actually used in the construction of an
assembly and also do not show on the BOM. An example of a reference part would
be the cardboard boxes in the assembly drawing of a packing machine. They are
shown (using the heavy dashed lines) for reference only. They are not actually
part of the machine.

Phantom (sub)assemblies are useful when you want the BOM to always blow through
the subassembly and show the components within. This would be the case with the
coupling assembly.



Dan_Inv9_sp4 wrote:
> 2008
>
> Detailed explanation: coupling with a set screw, I had the two halves and the insert in one assembly but I would prefer not to have a different part number for each possible combination of hub sizes (and fits etc.) but now the screws that are not purchased separately are in my bill, so I tried making them reference.
>
> Simple question: How do I keep something out of my bill without it bleeding through everything in a heavy dotted line.


--
Bob Wiley
Mechanical Designer

IV 2009 SP-
MDT2009 SP-
Vault 2009
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, 256 Mb, driver 6.14.11.6250, Full hardware accelleration
Spacemouse Classic serial, Acad-addin 3.2.8, 3DxWare 5.9.2, Firmware 5.49

[dan_inv09]

As I was reading I was going to reply and tell you That it is a content center screw that I might use somewhere else so I can't make it phantom. The reference part settings in the view dialog work great, now I just have to figure out how to make it default to those settings. And I'm not quite sure if it is a good thing that it carried through to the other views.

For now I'd rather not start littering my projects with copies of standard fasteners. Your way will work great for some special part, or in a special case though, so thanks.

[Anonymous]

Thanks for the response. I like your logic. I don't like duplicate files
floating around either.


I don't understand why Autodesk limited us to just two choices for parts at the
assembly level: "Default" and "reference". It seems, for me anyway, that
reference parts are rarely needed. Phantom parts are very common.

Maybe this should be on the wish list: Setting parts to phantom BOM structure at
the assembly level.



Dan_Inv9_sp4 wrote:

> As I was reading I was going to reply and tell you That it is a content center screw that I might use somewhere else so I can't make it phantom. The reference part settings in the view dialog work great, now I just have to figure out how to make it default to those settings. And I'm not quite sure if it is a good thing that it carried through to the other views.
>
> For now I'd rather not start littering my projects with copies of standard fasteners. Your way will work great for some special part, or in a special case though, so thanks.


--
Bob Wiley
Mechanical Designer

IV 2009 SP-
MDT2009 SP-
Vault 2009
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, 256 Mb, driver 6.14.11.6250, Full hardware accelleration
Spacemouse Classic serial, Acad-addin 3.2.8, 3DxWare 5.9.2, Firmware 5.49

[Inv_kaos]

I sometimes find that I need to adjust the margin too, to get the desired result. May just be me...

_____________


"It seems, for me anyway, that
reference parts are rarely needed. "

Have you ever made a skeletal model? How did you remove your master sketch part from the BOM?

Regards,
Stew

[dan_inv09]

But your master sketch doesn't lay over everything in big black dotted lines, does it? (Of course thanks to Andrew, I now know how it's supposed to work - I guess I need to try to pay attention to the "what's new".) And a different "Non-BOM" part would also work for sketch only parts as well as solids.

[Inv_kaos]

"But your master sketch doesn't lay over everything in big black dotted lines, does it?"

I was actually responding to Bobs comment, not your question about that part. Also it is not a new feature, it has been there as long as I can remember.

Regards,
Stew

[Anonymous]

Can't answer. I've never done anything with skeletal modeling. I assume the
master sketch is tagged as a reference part. Still, if we had complete control
of the BOM structure at the assembly level it would cover all bases.

Inv_kaos wrote:
> I sometimes find that I need to adjust the margin too, to get the desired result. May just be me...
>
> _____________
>
>
> "It seems, for me anyway, that
> reference parts are rarely needed. "
>
> Have you ever made a skeletal model? How did you remove your master sketch part from the BOM?
>
> Regards,
> Stew


--
Bob Wiley
Mechanical Designer

IV 2009 SP-
MDT2009 SP-
Vault 2009
XP Pro 2002 SP2
Dell Precision 650
Dual Xeon 2.40 GHz
2.00 GB RAM
Quadro FX 3000, 256 Mb, driver 6.14.11.6250, Full hardware accelleration
Spacemouse Classic serial, Acad-addin 3.2.8, 3DxWare 5.9.2, Firmware 5.49

[dan_inv09]

I was just saying that I though he meant that extra baggage comes along with "reference" when he (we) just need to not count certain parts.


I'm trying to remember if BOM was there in 9, and if so, how I managed to avoid knowing much about it. We skipped 10 and 11 (but as soon as I finish my current project we're going to 2009, yay) and we haven't had a class since 5.3.
Plus it's not so much how new it is as it is about much I knew about what it could/should do before I tried using it.