Hello, Lin, thank you for the input.
But I need to see Parts only. No assemblies should be in the BOM, only the parts (part files) should be visible there, but if the part has weldment cuts - then instead of that part, there should be a cut list items instead.
Ben, from your description I think you could make use of Intended bom with detailed cutlist. You'll have to use the dissolve option to dissolve the weldments or subassembly and show only the parts. Check the pictures below
this is what bom looks like before dissolving.
this is after dissolving the weldment. It shows all the cutlist items separately.
You can dissolve all the weldments and subassemblies in your main assembly bom and its going to show only the parts and cutlist items. I guess that's what you're looking for.
Hello Krishna, thank you for the detailed post.
The problem I am trying to solve here is that the policy of our company forbids using multibody parts. If a part has multiple bodies, then it should be the assembly, not the part. Unfortunately for me now, Solidworks is to have the default strategy for making weldment structures (as well as forms for casted parts) of making all structure as a one multibody part. It is really convenient work with this way for an engineer, who building the structure inside the computer, but the guy who is cutting the parts with the saw, as well as the weldment guy who is connecting the structure items, this brings a confusion - why all the assemblies are assemblies, but the assembly of the profile members ("Cut list items" in Solidworks) is the part?
As much as I tried to convince my manager to make an exception for welded structures of profile members, explaining the policy of Solidworks on the software level, it was not allowed. And on some level I must agree: I can explain this system to a few welders in my company, but if we are ordering the structure to be made outside our company, I'll have to do it every time to each subcontractor. Furthermore, this way brings issues when passing needed profiles to the purchase guy, etc.
Krishna, your suggestion is not acceptable, because "Intended" type of BOM has assemblies in it. I need "Parts only" type of BOM for exporting the list of items for purchases. Following your method, I should dissolve weldment part, but then I should hide all rows containing the real assemblies.
It would be perfect, if "Parts only" BOM type would have a "Detailed cut list" possibility and "Dissolve" possibility for the weldment part. In fact, I will put an enhancement request for this, I can not be the only one who needs it.
For the time being, I will use another solution. I will use "Save bodies" feature in the weldment part, creating a separate part for every cut list item. The "Save bodies" feature is also able to automatically create an assembly, which is the same as the parent weldment part. So I will have two objects, looking the same: the "part" file with all the structure, and the "assembly" file with separate bodies. This way I will get the benefits of easy editing (e.g. one click will change the type of all tubes), corner treatment etc. The parent "Part" will be "Envelope" used for construction. This will be the easiest way I guess ...
After working some more time with this issue, I found out that the best solution is not to use "Save bodies" feature on the cut list, even though it has the possibility to automatically create an assembly. In fact, I think nobody should ever use this function, here is why:
1. You can not normally edit the feature. For example, one more tube is added to the model. If you edit your "Save bodies" feature, and mark all of the bodies, including the newest one, it will save all of parts newly. This means, that internal ID of them will be changed, and any features you had in your parts will be gone. This is can not be undone.
2. The same scenario is when (lets say a new user with less experience) tries to save this new body separately. He edits the feature, and sees that all the parts have already been saved. He also knows that saving all the parts again will save all parts again, so any features on part level will lose it's references. So he wants to save only the last part: he checks it, clicks save. And now ALL of the other parts, except he save lastly, lose their relation to the parent part file. It is like they were never saved: the part file is not deleted from the disk, features are not deleted from the feature tree, but all the relations are gone. Even all the solid bodies are gone. And there is no way to undo that.
3. The third bad thing, although not as bad as the first two, is that it is "risky" to edit the saved parts list. If you edit one part on the edit feature window, and say you change the name of the part (leaving all other parts unchanged), all the other parts are saved again when you click OK, so you lose any feature references in each part file, except the main body.
This being said, I strongly advice to use the "Insert -> Part" command instead "Save bodies" feature, like described in this video:
(the time is 25:00, although there are 3 more techniques described in this video just before mentioned time, that are worth seeing)
"Delete body" feature now has the "Bodies to keep" possibility, meaning you only have to select the needed body, instead of selecting bodies you want to delete. This makes working much faster. Besides, this way all the structure has the same origin, although consisting of many different parts, so all parts can be mated to origin.
The Insert>part command can import also skeches, planes, cosmetic threads from hole wizard, and this feature can be perfectly edited. Meaning you can always and safely edit the body you want to have in each part (be editing "delete body" feature), you can edit what you want to import, etc.
If you have the same pipe twice in you weldment structure, you can create different configurations in the same part, by having different "delete bodies" commands suppressed. This way, you will have exact parts at exact locations with the goods names (you don't have to mate anything in assembly, except the origin).
Finally, ticking the "Display all configurations of the same part as one item" in the "Parts only" BOM makes your BOM the correct sense.
However, this is only a workaround. Having the "Show detailed cut list" in "Parts only" BOM with addition to the possibility to "DIssolve" the parent part would be a huge time save. I have submited an enhancement request for it, so please vote for it if you find the feature missing also. The ER number is : 1-8241944586
You put a lot of great information in this post