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BOM

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Message 1 of 17
jacornej
770 Views, 16 Replies

BOM

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.

16 REPLIES 16
Message 2 of 17
harco
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.

Message 3 of 17
jacornej
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.

Message 4 of 17
harco
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

Message 5 of 17
jacornej
in reply to: jacornej

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

Message 6 of 17
jacornej
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.

Message 7 of 17
harco
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.

 

Message 8 of 17
jacornej
in reply to: jacornej

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

Message 9 of 17
harco
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.

Message 10 of 17
jacornej
in reply to: jacornej

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

Message 11 of 17
harco
in reply to: jacornej

I don't know why it won't let you demote CC parts but we usually only use custom saved CC parts and don't use CC as such.

From what I've seen of CC parts they are mostly uneditable.

There may be a lock on CC parts which limits what you can do.

It may have something to do with tube and pipe, design accelerator, frame generator, bolted connection, this type of thing, they all tend to lock things down into their own assemblies.

Also patterns don't demote easily, normally have to destroy and rebuild.

 

Take a copy of the top level to try things out.

Select as much as you can demote to see what you would need to add to the sub in the way of CC parts, hopefully it's just a couple of joints.

Hope this helps some.

 

Message 12 of 17
jacornej
in reply to: harco

Well thanks for the help. I think for this one im just going to make a custom tables in the idw's. It was a learning experience, I now know what not to do

Message 13 of 17
guyh
in reply to: jacornej

Not sure how well this would work for you but how about setting all the other parts etc to Reference within the BOM, then when you create your drawings and parts list they should not be included.  You may need to manipulate how the referenced parts are displayed within the drawing to remove them but this should differentiate them from the main pipes.

 

cheers,

 

Guy

AutoCADM 2011 SP2
Inventor Pro 2011 SP2
Message 14 of 17
jacornej
in reply to: harco

If I do it that way it changes the BOM of the assembly file, which alters to qty in my other drawings

Message 15 of 17
jacornej
in reply to: jacornej

I found a pretty simple solution to my problem. I just save another copy of my main assembly, grounded all the parts of a certain pipe run and deleted everything else. Then I brought that in to the main assembly.

 

Another question I have is if I can combine pipe parts in the BOM, for example in one pipe run I use all 2in pipes. Inventor lists each section of pipe as it own part. Is there a way I can combine those together and get an overall length on the BOM.

Message 16 of 17
guyh
in reply to: jacornej

Not pipes but this blog post (great blog as well it should be said) may give you some ideas.

 

http://inventortrenches.blogspot.de/2011/03/understanding-autodesk-inventor-frame.html

AutoCADM 2011 SP2
Inventor Pro 2011 SP2
Message 17 of 17
jacornej
in reply to: guyh

I found of way of grouping them in the parts list by substituting the part number column with the stock number, but everytime I found a solution another problem comes up. When I group them together it doesn't give the group an item number.

 

For example let say I had 3 pipes with item numbers 1, 2, and 3. When I group them it makes a new row and in the item number column it shows like this (1,2,3,) is there a way to give this group and item number

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