Inventor General Discussion

Reply
Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 1 of 17 (430 Views)
Accepted Solution

BOM

430 Views, 16 Replies
10-04-2012 01:01 PM

Ok, I was giving an assembly with a lot of piping in it, but the piping wasn't done using the Tube & Pipe.

 

I need to make a drawing of the piping with a BOM. I made an ISO view and turn off the visiblity of the parts I didn't need. 

 

My question is if there is way for the BOM to only show the visible parts in my drawings. I know in iAssemblies I can exclude the parts I don't need, but that would take awhile considering there are over a hundred parts in my assembly. I really don't want to redo the piping mainly because of my inexperience with Tube & Pipe.

*Expert Elite*
harco
Posts: 879
Registered: ‎02-16-2006
Message 2 of 17 (418 Views)

Re: BOM

10-04-2012 01:43 PM in reply to: jacornej

If you set up a view rep in the assembly model you should be able to select the view rep in the part list in the drawing to show only parts included in the view rep.

The BOM will still show all the parts.

I don't have tube and pipe but I assume the view reps work the same as a normal assembly.

Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 3 of 17 (408 Views)

Re: BOM

10-04-2012 02:49 PM in reply to: jacornej

Ok I tried that but the Part List still shows all the parts.

 

The only way it doesn't is if I change the BOM Structure to Reference, but then it changes it in all the view reps.

*Expert Elite*
harco
Posts: 879
Registered: ‎02-16-2006
Message 4 of 17 (390 Views)

Re: BOM

10-04-2012 11:40 PM in reply to: jacornej

You will need to set the part list filter,see image

Select the view rep with the visibility of parts you require.

 

PART LIST FILTER.png

Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 5 of 17 (375 Views)

Re: BOM

10-05-2012 06:26 AM in reply to: jacornej

Thank you so much, you just saved me alot of time.

Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 6 of 17 (326 Views)

Re: BOM

10-08-2012 10:08 AM in reply to: jacornej

Ok, I didn't realize this until now. But the BOM still shows the qty for the entire assembly.

 

For example in the piping assembly I only have 7 elbows, but the BOM say I have 22, which is the qty for the entire assembly.

 

Is there anyway to filter that out too.

*Expert Elite*
harco
Posts: 879
Registered: ‎02-16-2006
Message 7 of 17 (317 Views)

Re: BOM

10-08-2012 11:14 AM in reply to: jacornej

Sorry, no, that's the one drawback with this method.

Lots of folk have complained about this.

Quantity stays true to the BOM not the view.

Only way is to highlight Qty beside balloon with text or a leader, or override balloon Qty (this is possible but a bit convoluted http://forums.autodesk.com/t5/Autodesk-Inventor/Balloon-quanity-question/td-p/2590146/highlight/true...

If you override the part list Qty it will affect the related Qtys in all part lists in that idw file.

 

It may be easier to split up the large assembly and demote to assemblies you require then views and Qtys will line up.

 

Sorry can't be of more help.

 

Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 8 of 17 (308 Views)

Re: BOM

10-08-2012 11:47 AM in reply to: jacornej

By spilt the assemblies, do you mean just recreating seperate sub-assembiles

*Expert Elite*
harco
Posts: 879
Registered: ‎02-16-2006
Message 9 of 17 (293 Views)

Re: BOM

10-08-2012 01:08 PM in reply to: jacornej

In a way yes, but you shouldn't have to recreate them.

In the top level, if you select all the parts which you want to be in a sub, you can right click, then demote them and create a new sub assembly.

If you do this as one step most of the constraints should hold.

 

I sometimes do this for hydraulic hose assemblies.

Place and constrain the ends in the top level,

Create the hose and line up with the ends,

Once I'm happy, demote the ends and the hose together to a hose assembly.

Contributor
jacornej
Posts: 18
Registered: ‎09-12-2012
Message 10 of 17 (290 Views)

Re: BOM

10-08-2012 01:17 PM in reply to: jacornej

Ok, but its not allowing me to demote parts from the content center

Announcements
Are you familiar with the Autodesk Expert Elites? The Expert Elite program is made up of customers that help other customers by sharing knowledge and exemplifying an engaging style of collaboration. To learn more, please visit our Expert Elite website.
Need installation help?

Start with some of our most frequented solutions or visit the Installation and Licensing Forum to get help installing your software.