Cut parts, PDM & BOM

[berg_lauritz]

Here is something our department was discussing the other day on what to do and we have multiple solutions but neither seems to be appropriate. How do you handle simple cut parts through PDM/BOM and in SolidWorks?

We do have different simple cut parts. They are only cut to length (also also have parts that are cut in 2 dimensions but let's not start with those):

1. metal tubes/rods/channels
   • pre-defined profile (i.e. 4"x4"x.25")
   • comes in pre-defined lengths (i.e. 12ft)
   • can be modified/bent accordingly
   • has only one color/finish to it
   • structurally important to have the correct material strength
2. lumber
   • pre-defined profile (i.e. 4"x2")
   • comes in pre-defined lengths (i.e. 8ft)
   • sometimes has a different finish/color
   • structural impact is minimal - the specific material (wood) is interchangeable
   • can not be bent/curved
3. edge banding
   • pre-defined shape that can vary from year to year (i.e. radius/thickness change)
   • comes in rolls
   • different colors
   • no structural impact
4. galvanized coil
   • pre-defined shape (i.e. 16ga 75mm)
   • comes in rolls
   • can be easily bent to shape

Now we want to properly implement those parts into our models and into PDM and our BOM. We thought about the following:

1. Everything (each length) is a real part & it does get a part number
   • Pros
     • We can search for each part # through PDM - we get a nice 'where used' & a great treehouse view
     • straightforward to handle in BOM
     • automatically bent parts (i.e. through laminates) are easy to implement properly into the assembly (because you can just link them with an external reference into that assembly)
     • have a specific drawing for each part
     • PDM data cards are available for every part
     • Straightforward
   • Cons
     • If i.e. the shape changes we'd have to replace EVERY part # that will be affected in all our assemblies
     • more work to make all the drawings (all the lengths...)
     • changes within PDM have to
     • can be hard to keep track of all the sizes/variations of all those parts
     • copying them over can lead to unwanted shared external references (if those are used) for those laminated parts - re-usability is dangerous
     • if no external references are used (example galvanized pieces in laminates) it is a lot of work to bend parts properly again just because they moved a little bit in the laminate
2. Drag in a design library part with pre-defined properties & make it virtual according to the length/bending you need
   • Pros
     • No searching for lengths is required because the length will be defined after dragging it in
     • Can be easily referenced to the assembly it is in without having to fear any repercussions (bending it & moving it is super easy & straightforward)
     • Only one drawing can be used/has to be maintained (with a variable for the length in it)
     • The design library part has only one PDM data card
   • Cons
     • Virtual parts have no PDM data-card which can be modified within the assembly
     • The PDM data card is only for one length
     • You can not really do a 'where used' in PDM for those virtual parts, esp. no treehouse view
     • Any revision to a profile would require to change all virtual parts individually
     • Any change to the custom properties would require to change all virtual parts individually
     • Copying that assembly would mean that changes on those standard parts are not automatically tracked (because they are virtual parts...)
3. Have one part in the design library that has multiple configurations & drag it in & select the configuration to work with this
   • Pros
     • Maintain only one part
     • The PDM data card has all the lengths in it - only maintain one data card across everything
     • A 'where used' is easily possible - also for lengths - with a nice treehouse view
     • With a design table maintaining all the custom properties across those configurations is easily possible
     • A profile change as a review is easily possible - after all it's just one part that has to be changed for all the configurations
   • Cons
     • Configurations are heavy on resources & it may slow down our models
     • No possibility of automatically bending those parts (no external references possible for laminated parts) - thus every single part that needs a reference HAS to be virtual or a new part # to be properly aligned in a laminate
     • i.e. Edge banding can only have lengths in it but no shapes/curves without making it virtual
     • PDM can not (?) automatically assign each length (configuration) a part number - can be done within the design table though
     • if each configuration has its own part # many drawings have to be maintained - that can be automated with PDM though

(I'll interrupt myself here, this post is already way longer than it was supposed to be, I did not really even touch the BOM part here with the colors etc...)
What do you guys do?
Do you have experience with this?
Do you add part intelligence for better traceability?
Do you derive those parts to 'get the best of all worlds'?

[bnemec]

Where I work every part has a part number, can be used anywhere, may be revised, likely very similar to another part. Also, parts have an undefined life span; 20+ years of use is not uncommon.

For the most part our packaging is not really engineered (although it should be) so we do not have models for that stuff. Exceptions are customer specific returnable crating and some others. We do not model soft trim (seat covers).

We use your option number 1.
- do not have external refs, they would (and have) cost us dearly.
- updating where used is a big job; we cannot understand how PDM has made it this far without a "Replace orupdate to new version all where used" function (Like SE Design Manager has)
- we do not have very many parts that change shape based on where used. We use A LOT of flexible/adjustable assemblies. Examples, tracks (for/aft rails) recliners, suspensions, gas springs, dampers, and yes springs (not ideal but it seems to be the least bad option)
- wire harnesses, hoses, etc are modeled to make a decent print but seldom actually routed in the model.
- weldments are modeled as assemblies, not as multibody parts.
- one part number per file.

option 3 comment: I'm working now on taking ALL of our hardware parts out of a few configured files because of several reasons. The last straw was Where Used in PDM couldn't do what we needed. Mostly because the where used were likely referencing old version of the configured part file (because it changes a lot as we add new hardware or revise existing) Now, in the where used the user must first select the version, then the config, there is no option to show the where used of all versions of a specific config.

One thing you didn't mention that hopefully isn't a problem for you, is are your CAD Assemblies structured according to manufacturing bom structure? We used to do that but now that assembly and inventory control started some drastic changes we are diverging in the assmebled part numbers. What we call "atomic" parts, things that cannot be taken apart or sub-kitted such as weldments or press in studs we still match the manufacturing bom. Mostly.

[bnemec]

While working with one of our configured hardware files I was looking for a part number (config) on the data card and got to a point that I thought was worth sharing. The list of configs in our washer file which is by far not the largest. Also, I don't know how to search configuration list in Solidworks. If you know how, please share.

Edit, that screen shot is from a 43" display, 2160 pixels high, why the text looks so small.

[berg_lauritz]

...
We do not model soft trim (seat covers).
...

We are trying to get there and we have many things already modeled or at least partially implemented. This has been an incredible amount of work at first but the benefits are starting to show (more accurate jigs(!); advanced shapes; traceability; etc.) and we are happy with the results. But those parts usually NEED some kind of reference for us (it is designed to fit ONE special seat/cushion etc.).

We use your option number 1.
- do not have external refs, they would (and have) cost us dearly.
- updating where used is a big job; we cannot understand how PDM has made it this far without a "Replace orupdate to new version all where used" function (Like SE Design Manager has)
- we do not have very many parts that change shape based on where used. We use A LOT of flexible/adjustable assemblies. Examples, tracks (for/aft rails) recliners, suspensions, gas springs, dampers, and yes springs (not ideal but it seems to be the least bad option)
- wire harnesses, hoses, etc are modeled to make a decent print but seldom actually routed in the model.
- weldments are modeled as assemblies, not as multibody parts.
- one part number per file.

After typing this all out it seems like this is our best option to try things out. We can do it & if it fails we 'just' lost time for testing but we don't have to go back and fix 100 things. We can just go forward.

- updating where used is a big job; we cannot understand how PDM has made it this far without a "Replace orupdate to new version all where used" function (Like SE Design Manager has)

Yes, seriously wtf. I was expecting PDM to have this.

- we do not have very many parts that change shape based on where used. We use A LOT of flexible/adjustable assemblies. Examples, tracks (for/aft rails) recliners, suspensions, gas springs, dampers, and yes springs (not ideal but it seems to be the least bad option)
- wire harnesses, hoses, etc are modeled to make a decent print but seldom actually routed in the model.
- weldments are modeled as assemblies, not as multibody parts.

We use some flexible assemblies - and we want to use more to get rid of some headaches that we get after building the first units...
Our plan is to have them in 3D - many of our changes/headaches come from wiring/plumbing not being properly aligned and/or measured. We did some testing and those units work way better!
We used weldments only to test the functionality and after going through PDM we won't use them. Not enough benefits for us!

option 3 comment: I'm working now on taking ALL of our hardware parts out of a few configured files because of several reasons. The last straw was Where Used in PDM couldn't do what we needed. Mostly because the where used were likely referencing old version of the configured part file (because it changes a lot as we add new hardware or revise existing) Now, in the where used the user must first select the version, then the config, there is no option to show the where used of all versions of a specific config.

Due to the nature of our shaped parts this is probably not for us anyway. And your comment does not give us any more hope of doing it this way. Thank you for the input, @bnemec !
We are struggling currently with this in PDM because we have

• CNC/Finished version for our parts for our edge banding - we design the part to fit & usually our edge banding 'cuts off' the part that it adds onto the part. This does not work with every part though & seeing which parts have edge banding is also beneficial. Having single part numbers for this creates a high workload for almost no benefit though. So we are probably going to use configurations & maybe even cut lists. That's one of the parts I did not touch
• Bent/Flat version for our laminates - because laminates are a pain in SolidWorks. We have yet to find a better way.

One thing you didn't mention that hopefully isn't a problem for you, is are your CAD Assemblies structured according to manufacturing bom structure? We used to do that but now that assembly and inventory control started some drastic changes we are diverging in the assmebled part numbers. What we call "atomic" parts, things that cannot be taken apart or sub-kitted such as weldments or press in studs we still match the manufacturing bom. Mostly.

Yes, they are mostly structured as to what the manufacturing BOM is. This is also due to our system that does not allow parts to have multiple routing points (i.e. part1 can not go to station1 first & then to station2 in the system).
I am curious though now what you mean with 'atomic' parts!? Laminates i.e.? Or pieces that are always welded together?

[bnemec]

We are trying to get there and we have many things already modeled or at least partially implemented. This has been an incredible amount of work at first but the benefits are starting to show (more accurate jigs(!); advanced shapes; traceability; etc.) and we are happy with the results. But those parts usually NEED some kind of reference for us (it is designed to fit ONE special seat/cushion etc.).

Due to the custom nature of our products each cover pretty much goes to one sku/catalog number. Often the cover pattern/logo/color is the only difference between a group of SKUs.

After typing this all out it seems like this is our best option to try things out. We can do it & if it fails we 'just' lost time for testing but we don't have to go back and fix 100 things. We can just go forward.

That's good for you, we would likely need to go fix them.

Yes, seriously wtf. I was expecting PDM to have this.

Right! I don't think the intent of the foundation of PDM was to support parts that live forever. I don't know if it's a language translation thing or intent, but in PDM SQL folders are called projects. I really get the feeling the PDM was built for the use case of a product that has a project folder structure with all the parts in that structure and those parts are all unique to that project. Anything that is used everywhere are OTS/purchased parts or Standard Parts Library so they get lumped into a different category and workflow than the projects. When a project is done it's done. The next project is ground up or a Copy Tree of the other Project. Then to avoid naming conflicts the folder and file templates came along. It wouldn't make sense to replace a part from one project to some other project or to even use a part outside of it's project folder structure. The next frequent comment I keep hearing is "well you don't revise your hardware or standard parts." That presumption just points back to why there is no replace all where used.

Also related wtf moment was when we realized there's no way to prevent users from transitioning to a state with special attribute (such as Obsolete) when there are where used that are not already in that state or the option to cascade UP the reference tree. Seems like a fundamental PDM concept. But, if everything is in a project folder structure for that product then it's not needed.

We use some flexible assemblies - and we want to use more to get rid of some headaches that we get after building the first units...
Our plan is to have them in 3D - many of our changes/headaches come from wiring/plumbing not being properly aligned and/or measured. We did some testing and those units work way better!
We used weldments only to test the functionality and after going through PDM we won't use them. Not enough benefits for us!

Flexible assemblies are where we use configs, Default is underconstrained as allows motion per design intent, then there may be a Top config and Bottom config that are more constrained to provide quick positioning in the upper level assemblies. That's just how we do it.

Due to the nature of our shaped parts this is probably not for us anyway. And your comment does not give us any more hope of doing it this way. Thank you for the input, @bnemec !
We are struggling currently with this in PDM because we have

• CNC/Finished version for our parts for our edge banding - we design the part to fit & usually our edge banding 'cuts off' the part that it adds onto the part. This does not work with every part though & seeing which parts have edge banding is also beneficial. Having single part numbers for this creates a high workload for almost no benefit though. So we are probably going to use configurations & maybe even cut lists. That's one of the parts I did not touch
• Bent/Flat version for our laminates - because laminates are a pain in SolidWorks. We have yet to find a better way.

It's tough when the part can be used anywhere and it needs to look good in the final model and drawing. Depending on what the part is we have used Virtual Component for something who's shape is dependent on the usage. Downside with this is it can mess up (or just make more complicated) the bom/parts list in eDrawings of the assembly or drawing. The other problem is if the part is changed then each VC may need updated.

Yes, they are mostly structured as to what the manufacturing BOM is. This is also due to our system that does not allow parts to have multiple routing points (i.e. part1 can not go to station1 first & then to station2 in the system).
I am curious though now what you mean with 'atomic' parts!? Laminates i.e.? Or pieces that are always welded together?

I borrowed the term from computing or database concepts where an action or event should not be interrupted from start to finish (my lay terms). I think they took it from chemistry where atomic means indivisible. We are using it to describe a part number that's made up of other part number(s) and the manufacturing bom structure isn't going to be in flux. Weldments for example aren't getting jostled around, we can keep our model structure in line with what manufacturing bom structure looks like.

For the sake of tac-times and other final assembly efficiencies Manufacturing Engineering has been making changes to the boms of assembled goods based on work center flows and WIP/vs stocked sub-kits. We cannot keep our models up to date with those changes. Some say there's no need to; problem is we have a constant flow of ECRs for these part numbers (some as customer requests, some manufacturing efficiencies, some sourcing changes, etc) that may or may not involve prints/model changes. So with no mapping between the cad structure (EBOM) and the Manufacturing BOM it becomes difficult to get a scope of work.

[Craig Schultz]

While working with one of our configured hardware files I was looking for a part number (config) on the data card and got to a point that I thought was worth sharing. The list of configs in our washer file which is by far not the largest. Also, I don't know how to search configuration list in Solidworks. If you know how, please share.

image.png

Edit, that screen shot is from a 43" display, 2160 pixels high, why the text looks so small.

After going down that road a loooong time ago, it's much easier to manage individual parts than all of those configurations. Certain things 20 years ago have scarred me for life. Just separate your hardware types into their own folders in PDM. You can also omit them from copy tree actions if you don't want to "switch" on the toolbox checkbox.

[bnemec]

After going down that road a loooong time ago, it's much easier to manage individual parts than all of those configurations. Certain things 20 years ago have scarred me for life. Just separate your hardware types into their own folders in PDM. You can also omit them from copy tree actions if you don't want to "switch" on the toolbox checkbox.

We failed to think about how putting hardware in their own folder would provide a means to prevent copytree. Ah well, we didn't give much thought to putting one part per file hardware in a special folder, as they are pretty much like any other part for us. Hardware all have a part number from the same list as all the other parts, and all our pre PDM files use the part number for filename. Our parts are very much not specific per project, so they just go in folders the make up every 1000 part numbers. So part number 123456 has file name 123456.par and is in folder CAD_Data/123/. So if we would take our existing hardware files (both the SE and SW files) and move them into a special folder they would appear as missing when the user is browsing the folder. Search tool would solve some of this but there are places where browsing is still faster.

[berg_lauritz]

Just a small update:

We are currently trying out to give everything a part# but for simple cut parts we omit the drawing (which is a blessing workload-wise).
Additionally we added some of our part numbers to the material database (i.e. for laminated sheets) and we just reference that within the part itself.

It's working pretty well so far but we need some more time to hopefully reap the benefits of this.

Many purchased parts needed optimizing though - so that they could be used properly with this. We still have some configurations for those parts (because they are bought as one piece but we only use parts of it sometimes i.e.).

I'll give an update probably in 2 months again.

Your input was as always very helpful!

@Craig Schultz, @bnemec - we put it into a different PDM workflow to automatically omit copying.

[Craig Schultz]

"we put it into a different PDM workflow to automatically omit copying." Yeah there's that too. I had former places set up for hardware workflow, the folder method, plus setting the toolbox check box. Someone was going to have to try reaaaaallyl hard to mess up a copy tree.

[berg_lauritz]

"we put it into a different PDM workflow to automatically omit copying." Yeah there's that too. I had former places set up for hardware workflow, the folder method, plus setting the toolbox check box. Someone was going to have to try reaaaaallyl hard to mess up a copy tree.

Yes, that was one thing we did right at the beginning. It's also easier to change things there (basically no review is needed after the first approval) (i.e. add ref. geometry etc.) for those parts and we don't do revisions on them at all.
I know it's dangerous to give those permissions - but our department is small & it works here.