Autodesk Inventor

[#1]

Hello

I am doing a .idw drawing of an assembly that I have several parts that I do not want to appear in the BOM parts list. I have therefore set these parts as Reference parts however this has caused them to appear as "hidden type" lines in the drawing and are even visable through other parts.

Is there any way to make these parts appear in the drawing "as normal" and not be listed in the parts list?

Thanks for any help

[#2 · Accepted solution]

"As normal", no... but, you can set some options for it on the "model state" tab when editing the view.

"Reference data - as parts" and "hidden line calculation - all bodies" will probably get something more desirable as you currently have.

[#3]

Actually thats exactly what I was after. Thanks very much

[#4]

Is there any way to do this for just one reference part but not all of them?

[#5]

The options mentioned only work on all reference parts in the idw environment.

What are you trying to accomplish exactly?

Maybe a different BOM state could help, or a different color style...

[#6]

What I have is an assembly using a couple of pneumatic cylinders along with a large frame that needs to be a referenced part.  The cylinders are a purchased part but I need them to function using limits, appear on the BOM so that our vendors will know the necessary specs for the cylinder, and look like a regular part on the drawing.  My solution is to create an assembly of each cylinder out of two referenced parts (plunger and housing) so that it does not create a BOM, then put the cylinder assembly into the larger assembly as a flexible part. 

This makes the cylinder assembly appear as a reference part on the drawing (thin lines).  I can sometimes fix this by selecting the lines and changing line style.  But this doesn't work when there are hidden lines or for sections.  I would like a way to make the cylinder act like a normal part even though it contains only referenced parts.

Thanks for any help

[#7]

There's a much easier way for you: make the cylinder assembly Purchased.  This hides the component parts from the BOM.  No need to use reference parts for this case.

To make it Purchased (or Inseparable), open the Document Settings, go to the Bill of Materials tab, and change from Normal to Purchased.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 1
Windows XP Pro 32-bit, SP3
HP EliteBook 8730w; 4 GB RAM; Core™ 2 Duo T9400 2.53 GHz; Quadro FX2700M
SpaceExplorer/SpaceNavigator NB, driver 3.7.18
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[#8]

I agree with Sam, the purchased state will accomplish what you want.

In my company we use cylinders in a similar way for movement, but we leave them on the "normal" state.

We can do this because we use "all levels" for our BOM and do not expand the cylinders to show their components.

(i realize we could set them to purchased, but we just never did since it doesn't matter that much for us.)

[#9]

In our case, we actually place separate parts lists for fabricated parts and purchased parts, and this is how we filter the lists.  Very convenient!

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 1
Windows XP Pro 32-bit, SP3
HP EliteBook 8730w; 4 GB RAM; Core™ 2 Duo T9400 2.53 GHz; Quadro FX2700M
SpaceExplorer/SpaceNavigator NB, driver 3.7.18
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[#10]

Thankyou for the input but it didn't work. The problem that we may be having is that we use Autodesk Productstream as our data managment program.  Productstream still shows the parts in the BOM and when I look at the BOM in Inventor it also shows all the parts.  Should the parts still be visible in the BOM in Inventor? Or am I running into an Inventor function that just doesn't work with Productstream