Inventor drawing BoM structure affects other drawings.

[NigelHay]

I have what I think is a glitch in Inv2015 as this did not happen in previous versions. I create an assembly & produce an assembly drawing listing all of the parts. I then use this assembly in a higher level assembly &, in the parts list call up the original assembly as a single item. I achieve this in the 1st drawing by setting the assembly BoM structure in the parts list to 'normal' so that all of the parts show. In the 2nd drawing I set the sub-assembly BoM structure in the parts list to 'phantom' so that the sub-assembly appears as 1 item.

My problem is that, when I change the BoM structure to 'phantom' in the 2nd drawing, it also changes in the 1st drawing so that the drawing parts list is reduced to 1 item. If I change the BoM structure back to 'normal' in the 1st drawing, it also changes in the 2nd drawing so that the single item expands to show all of the sub-parts.

Is this a glitch or am I doing something wrong?

[MartinBernat]

Hi Nigel,

I'm not sure how you set the BOM structure to 'phantom' in the drawing. If you achieve this using "Bill Of Materials" context menu, then you edit the assembly BOM and then both drawings get updated - this is normal behavior.

Martin Bernat,

Autodesk

[mcgyvr]

In the real world (and Inventor) a subassembly cannot be both normal and phantom.

A phantom is a non-stocking subassembly whos components get pushed up into the upper level assembly. 

If you create a drawing for this phantom subassembly and use that subassembly as the parent view all the components will show up in the parts list.

If you create a drawing of an upper level assembly that uses that phantom sub the components of that sub will show up in the upper level assembly parts list.

From your original description it actually sounds like you are also doing something wrong.

But the facts remain the same.. An assembly cannot be both phantom and normal in the real world.

[NigelHay]

Strange that I have not encountered this before, I'm pretty sure that I have had this set-up with other assemblies.

So, if the sub-assembly has to be either phantom or normal, not both, I still have a problem. I have one drawing which is a sub-assembly plus some parts in which I need all of the parts plus sub-assembly parts to show in the parts list. I have another drawing in which the same sub-assembly is incorporated into a larger piece of equipment so I want the sub-assembly to appear in the parts list as a single item. Can I achieve this?

[mcgyvr]

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@NigelHay wrote:

Strange that I have not encountered this before, I'm pretty sure that I have had this set-up with other assemblies.

So, if the sub-assembly has to be either phantom or normal, not both, I still have a problem. I have one drawing which is a sub-assembly plus some parts in which I need all of the parts plus sub-assembly parts to show in the parts list. I have another drawing in which the same sub-assembly is incorporated into a larger piece of equipment so I want the sub-assembly to appear in the parts list as a single item. Can I achieve this?

---

Again.. a sub cannot be both phantom and normal so in the real world what you seem to be doing is inconsistent practice that could cause confusion.

#1-The "proper" way IMO would be to have a drawing (or single sheet in a multipage drawing) for just the sub and its parts list will show all the components as usual. Then another drawing (or sheet) to show that assembly with the sub plus the "some parts" and that parts list would just show the sub and not its components plus the other parts.

#2-You could also just do a parts only parts list on the first drawing. 

#3-You could also just "demote" the sub in the first iam model to completely remove the sub and just show all its components thus loosing the link to that sub.

Personally I think #1 or even #3 is the "proper/consistent" way as if you can't have a sub be both normal and phantom I don't think you should ever show a drawing in that manner either. 

[NigelHay]

I agree that what I am doing is probably not best industry pracice but it is the situation that I inherited several years ago & the company now has 10,000+ drawings of parts & assemblies that have been configured that way so change is difficult. This is compounded by the fact that a large number of those drawings, whilst still in use, are in ACAD 2D format & others are in an older DOS based CAD format.

I see what you are saying with "if you can't have a sub be both normal and phantom I don't think you should ever show a drawing in that manner either" but that means that the software limitations are driving the business practice which is not good.

The practice here is that there is 1 top level assembly for each product even though that product contains sub-assemblies that can be used in other products. We then issue build instructions to the factory using works orders that are generated from an MRP software package. That allows us to break down the top level assembly into subs & re-combine them in different ways to create different products. This is done because we have a core range of base products but each of those products has several options so having a specific drawing for each variant would be onerous.

[warrentdo]

Hello,

I have the same problem.

Three conveyors all joined together, a conveyor line.

One main GA drawing showing all three conveyors in normal, BOM list all three.

Three separate conveyor drawings all showing each conveyor with the other two conveyors in reference so the drawing gives complete line.

It would be good if you could toggle to Phantom in the line drawing and normal in the drawing that you want to BOM off the parts.

Instead we have to create a shrinkwarp and insert that into the line drawing so that we can phantom it off. Bit messy.

Regards

Warren.

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[NigelHay]

In the drawing, bill of materials, you can set the other 2 conveyors to 'reference'. They disappear from the parts list & will appear as dotted outlines in the drawing.

[warrentdo]

Hello,

But that changed the other two drawing that use the same assembly.

The way around it is to create four separate assemblies! all the same apart from -

assembly one has all parts normal. this to be used in top level GA that only list 3 parts.

assembly two has part 1 normal part 2 and 3 ref. this is used in part 1 details BOM

assembly two has part 2 normal part 1 and 3 ref. this is used in part 2 details BOM

assembly two has part 3 normal part 1 and 2 ref. this is used in part 3 details BOM

This is crazy!

scream like I-assemblies

Regards

Warren.

[mcgyvr]

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@NigelHay wrote:

 but that means that the software limitations are driving the business practice which is not good.

---

No.. not a software limitation at all.

There are methods to achieve what you want..and I've already posted a few of them

But no matter what a single sub cannot be both phantom and normal. Its just plain WRONG.. its not a software limitation. Its how the real world works. The software follows that proper practice. 

I'd bet your MRP package doesn't really support that either.. it would be the first I've ever seen that does. 

You just simply cannot have a non-stocking sub and at the same time it be stocked.. Thats ALL phantom is.. a non-stocked subassembly.. or "built on the fly (as needed)"

But I really suspect you just don't understand the situation properly or how to apply the functions in Inventor or what options are available to get the desired outcome.

There is nothing wrong with having parts only parts lists in Inventor. (one that shows a subs components)

If you show me 2 real examples (autocad drawings or whatever) of exactly how you want it I will happily provide an example of how to properly do it in Inventor.. 

[mcgyvr]

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@warrentdo wrote:

Hello,

I have the same problem.

Three conveyors all joined together, a conveyor line.

One main GA drawing showing all three conveyors in normal, BOM list all three.

Three separate conveyor drawings all showing each conveyor with the other two conveyors in reference so the drawing gives complete line.

It would be good if you could toggle to Phantom in the line drawing and normal in the drawing that you want to BOM off the parts.

Instead we have to create a shrinkwarp and insert that into the line drawing so that we can phantom it off. Bit messy.

---

I just don't understand why you guys are having problems 🙂 and I'm cranky today 😞

You have one drawing showing the whole conveyor line.. Its parts list is simply (Conveyor 1.iam, Conveyor 2.iam, Conveyor 3.iam).. Thats it.

Then assuming these conveyors are the same it just takes 1 more drawing using either conveyor 1 or 2 or 3 as the base view and placing a parts list for that..

That parts list will show (leg left, leg right, horizontal left, horizontal right, and the rollers) or something like that.

If they aren't the same then its 3 drawings 1 for each and each iam is used as the base view not the top level assembly. 

And keep remembering what a phantom really is.

A phantom sub is one that is not stocked and is built on the fly and its components are shown in the upper level assembly bom (pick list or whatever).

If you don't stock conveyor 1 or 2 or 3 (or have a seperate job order that builds them first) then they are phantom. 

[warrentdo]

I dont think that you have got my problem,

All conveyors/machines are different.

what I/client require is-

Ga drawing showing all three. This to be used in top level GA that only list 3 Machines top level.

Drawing for machine 1. machine 1 detailed in BOM machine 2 and machine 3 ref.

Drawing for machine 2. machine 2 detailed in BOM machine 1 and machine 3 ref.

Drawing for machine 3. machine 3 detailed in BOM machine 1 and machine 2 ref.

How do you do this from one assembly?

Regards

Warren.

[mcgyvr]

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@warrentdo wrote:

I dont think that you have got my problem,

All conveyors/machines are different.

what I/client require is-

Ga drawing showing all three. This to be used in top level GA that only list 3 Machines top level.

Drawing for machine 1. machine 1 detailed in BOM machine 2 and machine 3 ref.

Drawing for machine 2. machine 2 detailed in BOM machine 1 and machine 3 ref.

Drawing for machine 3. machine 3 detailed in BOM machine 1 and machine 2 ref.

How do you do this from one assembly?

Regards

Warren.

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I get it but don't understand why

Why must the other machines be shown as reference in the individual machines assembly drawings? 

Regardless of the answer because I expect it to be some silly company request..

I would simply place (for example) machine 2 and 3 into the iam file for machine 1 and set them as reference then use a design view rep to hide them in the upper level assembly.. bam.. problem solved 🙂

[NigelHay]

My problem is much the same as warrentdo's. I have a sub that I sometimes want to fully detail along with some additional parts & sometimes want to call up as a single item. I am aware that in other industries that would be done by having a GA drawing of the sub on it's own, then call that up into higher assemblies but that is not done in this company. Creating drawings for all of the subs would result in hundreds more drawings.

[warrentdo]

Its because they want to show continuity of the line and the checker needs to know that it all fits together.

I know its a real pain, but toggling ref on and off would work well in our scenario.

Regards

Warren.

[mcgyvr]

So it seems that my suggested method of including the other "associated" sub assemblies into each sub and setting them as reference and then using design view reps to hide those reference subs in the corresponding upper level assembly will work for both your situations.. correct?

[warrentdo]

Well yes, that is the way that we currently do it, but its very messy, its not ideal.

We need to create shrinkwraps of all assemblies and post them into other assemblies as ref.

We use lod 1 for assembly on its own so that we can build up a master line, LOD 2 for assembly with shrinkwrap refs use for detailing up the assembly with its ref parts.

That the whole point of this thread. its a crap way of doing it!

Toggling assys normal to ref within lod would be much better.

Regards

Warren.

[swalton]

Here is another idea. 

1. Make your GA assembly with all three conveyors.

2. Make your print for Conveyor 1.

3. For every view that shows Conveyor 1 and Conveyors 2 and 3, place the GA.iam.  Set your selection filter to edges and click on the Conveyor 2 and 3 entries in the model browser for that view.  Right click and set the properties to another line type, Dashed for example.

4. For every view of that shows only Conveyor 1, place Conveyor 1.iam

5. When you place your parts list, select Conveyor 1.iam not GA.iam.

6. Add balloons to the Conveyor 1 only views.  I think if you add balloons to the GA.iam views, IV will pull item numbers from the GA BOM, not Conveyor 1 BOM.

I don't know if this will be any less hassle than making substitute LODs and adding them to the individual Conveyor iams.  It will work better if you only have a few views that require the GA.iam.

[mcgyvr]

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@warrentdo wrote:

Well yes, that is the way that we currently do it, but its very messy, its not ideal.

We need to create shrinkwraps of all assemblies and post them into other assemblies as ref.

We use lod 1 for assembly on its own so that we can build up a master line, LOD 2 for assembly with shrinkwrap refs use for detailing up the assembly with its ref parts.

That the whole point of this thread. its a crap way of doing it!

Toggling assys normal to ref within lod would be much better.

Regards

Warren.

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>We need to create shrinkwraps of all assemblies and post them into other assemblies as ref.

No you really don't NEED to create shrinkwraps. Why can't you simply drop converyor2.iam and conveyor3.iam into converyor1.iam and simply set 2 and 3 as reference?

subs or parts can be reference in one assembly and not in another. 

[warrentdo]

Hello, admittedly I don't need to create the shrinkwraps but in this occasion because I had to make 4 seperate assemblies it was worth while to keep the speed up. The whole point is that I had to create 4 seperate assembles when really I only want one that I can use in multiple drawings and just toggle the state/lod. Yes I can save out 4 times then change but I still have 4 assemblies to look after. 4 to modify if I add or edit the line.

Regards,

Warren.