Suppressed Parts IN Part List or BOM

[Anonymous]

I have read through many of the posts regarding this subject in several of the dicussions but it doesn't seem very easy or straight forward how to make a part not show up in either the cut list or the BOM.  I am a newby in Inventor but well versed in another program who's initials are SW 

If I am not mistaken, in the other CAD program if you suppressed a part from an assembly it would make the part "go away" and also remove the part from the BOM or adjust the quantity of parts if there were more than one of the supressed parts on the model and drawing. I do know for certain you had several options when you wanted the BOM to behave a certain way. Such as whether to show parts in the BOM individually or give a total qauntity if there were more than one etc, Supressed in SW was very different than "Hide" Hide was more like "Visible" in Inventor but supressed made the model and drawing completely ignore the supressed part basically like it did not exist anywhere while supressed. But when unsupressed it would afdjust the BOM, the model etc. It sounds like is that supressing a part in Inventor is really not much different than turning off the visibility?

So is there an easy way in Invenntor to make a part be completely ignored anywhere it was used in a model, partss list or BOM without actually deleting it or running complex rules and Ilogic etc.?  I understand that parts list refers to  either a drawing or an assembly and the BOM refers to the other. Not sure which though.

Any help on this would be greatly appreciated. 

[Cadmanto · Accepted solution]

Having worked in Solidworks myself for 12 years, and now in inventor the last 4.5 years, it took me a while to get used to the suppress feature in Inventor.

Basically in Inventor when you suppress parts in the assembly it creates what is called a levels of detail.

When you create an LOD (likem or hate them) it will change the quantities in the parts list.  But, with that said, the parts list has to represent the correct LOD represented by the associated view attached to the parts list.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[salariua]

Parts List, Material List,... are used in the drawing

BOM is used in the assembly

However you can access the BOM from the drawing but not the Parts/Material List from the assembly.

[Anonymous]

Thanks for the advice. So my understanding is that there is now way to simply click on a part and wave a magic wand over it and make it dissappear from  model/assembly or the parts list whether in the the drawing or the BOM in the Assembly  Guess I better brush up on the LOD  and iAssemblies.

Thanks for all the input!

[salariua]

There are ways of doing this but it all depends on specific cases (test each and see which works for you)

you can set that component as reference (BOM or assembly browser), which will not include it in mass calculations, center of gravity, etc. and it will show it in doted line in the drawing (this can be changed to show as normal parts).

you can also set it to phantom (BOM), which will include it in mass calculations, cog, etc. and the part will show as normal in the drawing, however, if this is an assembly it will show it's children promoted to a higher level. thik of this as a container of parts. 

you can also edit the parts list (drawing) and right click on an item then choose Visibility to toggle it on/off.

[Anonymous]

Thank you.

What we are dealing with is a rather simple assembly, a cabinet. This cabinet can be a right handed cabinet or left handed cabinet. The only difference between the two is one individual part.  For a left the part has a miter on the left hand and for the right it has a miter is on the right end. So in our assembly we have both parts in the assembly. Buit they bot show up in the parts list when we suppress either of them. For appearabce that works and so would visiblity. What we are looking for is a way to suppress or something that would adjust the parts list in the drawing.  

So as far as whether we see it or not we have that covered it is n ow just the parts list and what it shows as being used for either left or right. Hope this makes sense.

Thanks

[mcgyvr]

Reference = a part or assembly you want shown in the assembly but don't want it to be included in the BOM/Parts list.. For example.. If you were designing an assembly fixture for a product.. The product itself would be set to reference so it shows in the model but obviously should not be shown in the BOM for the assembly fixture.

Phantom = non-stocking built on the fly subassembly. The children components of the phantom subassembly are promoted into the upper level bom and the phantom sub part number is not shown.

iassemblies= allow you to have one assembly file to show multiple configurations of a product. Example: a machine thats available with different options and each "member" is a sellable part number and these assemblies are "like" enough to allow them to be maintained in one "iassembly factory" file..

iparts = allow you to have one part file to show multiple configurations of a part. Example: a table leg thats available in multiple lengths and these parts are "like" enough to allow them to be maintained in one "ipart factory" file instead of multiple single parts each with its own file. 

I believe iassemblies are referred to as "configurations" in Solidworks..

So far the solution to this post sounds like iassemblies is the way to go..

1 "member" has certain parts suppressed so they don't show up in the model/bom/parts list for that specific assembly part number

and another "member" has those parts unsuppressed so they do show up in the model/bom/parts lists for that specific assembly part number.

[mcgyvr]

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@Anonymous wrote:

Thank you.

What we are dealing with is a rather simple assembly, a cabinet. This cabinet can be a right handed cabinet or left handed cabinet. The only difference between the two is one individual part.  For a left the part has a miter on the left hand and for the right it has a miter is on the right end. So in our assembly we have both parts in the assembly. Buit they bot show up in the parts list when we suppress either of them. For appearabce that works and so would visiblity. What we are looking for is a way to suppress or something that would adjust the parts list in the drawing.  

So as far as whether we see it or not we have that covered it is n ow just the parts list and what it shows as being used for either left or right. Hope this makes sense.

Thanks

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You posted this as I was writing my last post.. And based on this iassemblies is 100% the way to go..

[salariua]

This is simple and for this you can use design view representations.

If you were trying to hide a number of occurrences like say: showing 3 bolts from a total of 5 then you would need iAssembly.

While this can also be solved with iAssembly I would use design view representations.

Create two view representations, Left and Right. In each turn off the visibiliy of those mittered parts.

Open the drawing and edit the parts list, click on filer and choose Define Filter Item "Assembly View Representation", then choose the correct represetnation in the box bellow.

[mcgyvr]

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@salariua wrote:

While this can also be solved with iAssembly I would use design view representations.

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I wouldn't.. 

This is 100% a case for an iassembly.. Thats what its 100% for.. 

Using design view reps is a workaround IF we didn't have iassembly functionality.. But we do.. so use it. 

I could hammer in a nail with my metric adjustable wrench.. But why.. I also have a hammer in my toolbox. 

[Anonymous]

Thank you for the advice. You are correct, in Solidworks they were considered configurations. You could make a simple light switch with the toggle in the up position for "ON" and another configuration with it down for "OFF".



Scott Pauley
Senior Design Engineer
Highland Ridge RV, Inc.
3195 N. St Rd. 5
Shipshewana, IN 46565
Phone: (260) 768-7771 Ext. 5186
Cell: (321) 298-5392
Fax: (260) 768-7410
E-mail: [email protected]

[Highland Ridge_Logo_w-quote]

[salariua]

It all depends on how much time you have for this. Is it a one time only? will this need changing in the future? Will others know how to handle iAssemblies to edit this.

Everything we do is pretty much custom and very rarely repeatable so that's why I would not use iassemblies but now he's got all options to choose from.

Editing a design view representation will get the results and that can be done by an inexperienced student/trainee.

[mcgyvr]

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@Anonymous wrote:
Thank you for the advice. You are correct, in Solidworks they were considered configurations. You could make a simple light switch with the toggle in the up position for "ON" and another configuration with it down for "OFF".

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That would be a "positional representation". 

An "iassembly" would be a simply light switch and a customer could buy one with a blue faceplate and red toggle or a red faceplate and blue toggle..

The toggles and faceplates would be created as an "ipart" with an appearance override for each colored member and the whole switch assembly as an iassembly with 2 "table replace" columns to switch between faceplates and toggle switch pieces..

Another example of an iassembly would be an Open Range 3X trailer from Highland Ridge RV.. One iassembly "member" would be the trailer with the 23 cubic foot fridge and the other "member" would suppress that fridge and then include the 12 cubic foot fridge and maybe a wooden blanking panel in the leftover space..  

[Anonymous]

You have hit the nail on the head. Can you contact me offline or is that forbidden?

Scott Pauley
Senior Design Engineer
Highland Ridge RV, Inc.
3195 N. St Rd. 5
Shipshewana, IN 46565
Phone: (260) 768-7771 Ext. 5186
Cell: (321) 298-5392
Fax: (260) 768-7410
E-mail: [email protected]

[Highland Ridge_Logo_w-quote]

[mcgyvr]

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@Anonymous wrote:
You have hit the nail on the head. Can you contact me offline or is that forbidden?

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me? (it helps to click the reply button by a specific users post to make it easier to follow.. Notice how your post says "in reply to" and its yourself so I'm not sure if you are referring to me or not..)

You can Private message me if you want..

You can also do "shoutouts" or whatver kids are calling it these days like this.. @Anonymous@ (start with the @ symbol and then users in this post will come up in a list that sends that person a special email letting them know you want their attention specifically)..

or

You could just continue the discussion here too which might be beneficial to others..

This is a peer-peer user forum (I don't work for Autodesk) so I/you can contact whomever you/I want.. They don't own me. muuhaaaahaha 

[Anonymous]

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@Cadmanto wrote:

Having worked in Solidworks myself for 12 years, and now in inventor the last 4.5 years, it took me a while to get used to the suppress feature in Inventor.

Basically in Inventor when you suppress parts in the assembly it creates what is called a levels of detail.

When you create an LOD (likem or hate them) it will change the quantities in the parts list.  But, with that said, the parts list has to represent the correct LOD represented by the associated view attached to the parts list.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

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I experienced that LOD does nothing to the part list or BOM as such, its only the View representations that can directly alter the part list in the drawings.

[johnsonshiue]

Hi! Indeed, LOD is a memory management tool. It does not alter the BOM and the PartsList. It only loads or unloads component documents from the memory.

Many thanks!

[cwhetten]

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@hashone wrote:

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@Cadmanto wrote:

Having worked in Solidworks myself for 12 years, and now in inventor the last 4.5 years, it took me a while to get used to the suppress feature in Inventor.

Basically in Inventor when you suppress parts in the assembly it creates what is called a levels of detail.

When you create an LOD (likem or hate them) it will change the quantities in the parts list.  But, with that said, the parts list has to represent the correct LOD represented by the associated view attached to the parts list.

---

I experienced that LOD does nothing to the part list or BOM as such, its only the View representations that can directly alter the part list in the drawings.

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As @johnsonshiue said, LOD does not alter the BOM.  The only exception is if all occurrences of a part are suppressed, then that line will be removed entirely from the BOM.  If some occurrences of a part are suppressed and some are not, the quantity in the BOM will be wrong.  LOD and suppression should not be used for BOM configuration.

View representations do not alter the BOM.  Making a part invisible does not remove it from the BOM.  There aren't any exceptions here--it never works that way.

What alters BOM is the property called BOM Structure.  BOM structure is discussed by @mcgyvr in post # 7 above.

If you intend to create a configurator using iLogic instead of iAssemblies, I recommend using visibility and view representations, but you must also set the correct BOM structure.  Otherwise your BOM will be wrong.

Cameron Whetten
Inventor 2018

[johnsonshiue]

Hi Guys,

Just to clarify the BOM behavior when a non-Master LOD is active. BOM table should never change regardless of all occurrences are suppressed or not. I am not aware of a workflow that a non-Master LOD can lead to BOM table change. There are only two exceptions. 1) The mass prop of the assembly can be computed excluding suppress components. 2) iLogic offers a function called IsActive(). When a given component.IsActive() equals to false, Inventor sets the component occurrence BOM attribute to Reference and then suppress the occurrence. This does lead to one occurrence deducted from the BOM table. But, in theory, this has nothing to do with LOD. You can manually change any occurrence to Reference and suppress it accordingly.

Many thanks!

[Ed__Jobe · Accepted solution]

In all this discussion, I'm still not sure of how to accomplish what I want. I have a part in an assembly, but some instances are suppressed for future installation. I want to exclude only the suppressed items from the BOM so the count for that part is correct. What steps do I need to take?