How do you handle standard parts in modified/deformed states?

[laukejas]

Hi, this is a generic question about standard part (library) management when these parts need modification or representation in specific shape in a project.

For example:
1. A bolt that has a hole drilled through it's shaft;
2. A normally round belt that is formed into a specific shape around pulleys;
3. A compressed O-ring;
4. A PCB board that has it's edge trimmed to fit in a very tight space;
5. A Li-Po battery with wires and connector sticking out of it, and these wires are bent into a specific location;
6. A threaded rod that has been trimmed in length;
Etc, etc.

These changes are easy to implement geometrically, but I am not sure where these changes should be done, considering that these are standard parts. These are the options I tried, but none of them are ideal:

1) Make a configuration of the part in deformed state (for example, O-ring in compressed shape). Unfortunately this can be really a lot of work if the part already has configurations (different sizes), so the number of configurations would be doubled. Also, deformation/modification might be unique project-specific (for example, specific belt shape around pulleys), and it wouldn't make sense to keep it as configuration inside a library part.
2) Use "Make Independent" option to create a clone of the library part inside the project directory, and then modify it for that specific case. Unfortunately this provides no parametric link to the original library part, so if it is changed (for example, Custom Property like Source is updated), it won't reflect in the project, and will have to be updated there manually. Also, it kind of creates file duplicates.
3) Insert library part into a new empty part, and make modifications there. This keeps parametric link, but sometimes deformation changes are very difficult to make without original feature history (for example, compressing an O-ring is easy with a simple Scale feature, but how would you change belt shape?). Also, this option is a bit annoying because I have to use Replace Component in the assembly every time to replace the library part with this modified version.

Currently, I mostly use the 3rd method, but I am looking for better options. How do you guys handle such cases?

[JSculley]

1. Create an assembly, insert the purchased part, make modifications there. This keeps the BOM correct. You buy part ABC123, you modify it to create part DEF246.

2. I'd use configurations, with the config name providing some sort of link to where it was used. For example, 'FOR ASSY ABC123'.

3. Configurations. I made my o-ring model from a revolved ellipse with configurations for all of the o-ring sizes by dash number. That way, I can tweak the dimensions for ID pressure, OD pressure or face seal applications. The nominal dimensions are the main config, derived configs for the others, which are added as needed.

4. See answer 1. Modified purchased part.

5. I would probably show the wires straight out in one config so that the wire length was obvious. Then use configs with the wires suppressed but the connector positioned via a Move Bodies feature. In the assembly where the part is used, use a virtual part for the wire routing.

6. We treat threaded rod and other materials available in various lengths as a raw material, so the drawing would show the rod with the hole and the material would list the threaded rod. A note on the drawing provides guidance on what could be ordered, but does not force it. If a 4ft rod cut into 4 1ft pieces is more cost effective, go for it, as long as the end result matches the drawing.

[Alin]

An interesting alternative is using the flexible component functionality. It is unexpectedly robust, fast and produces the expected results for most applications.

https://help.solidworks.com/2023/englis ... Redirect=1

https://www.javelin-tech.com/3d/solidwo ... omponents/

[Frank_Oostendorp]

"It is unexpectedly robust"

[dave.laban]

I'd answer the same as JSculley, with the exception of 3; I'd just leave the default size in the assembly and not care that there's a bit of interference in a face or two.

[Glenn Schroeder]

Are the changes you're talking about for a specific project, and you don't anticipate needing that file again? If yes, I'd recommend you copy it to the project folder, change the name, and then make your edits. Don't bother linking it to the original Part (for the first example you gave, it's not like bolt dimensions are going to change).

If you do anticipate needing it for multiple projects then I'd make it a configuration and leave it where it is.

[mike miller]

Keep assembly features in mind for use cases where material is removed. Here's a case we've had:

Collar A is purchased form vendor. In ASM123 one occurrence is welded as-purchased, another occurrence gets a tapped hole and grease zerk before being welded.
Our solution was to use the direct part file Collar A for the first occurrence, obviously.
For the second occurrence, we created a S/A with Collar A, added the hole with an assembly feature, and mated the zerk in place. This also served as a source for the machining drawing.

Use your head and think through the ramifications of each method.

[bnemec]

In our use case it winds up varying case by case as it affects and is dependent on several things. Every situation is a different compromise. Trying to shove every situation through the same process would be unacceptable most of the time. Following your examples in the list below. We do not have "standard parts" in the common definition; our entire data set is pretty much a parts library. Furthermore, MFG ENG will change the process over time for various reasons. What used to be an operation step, is sometimes changed to a new inventoried part number for example. So we then need to adjust our model structure for that.


1. A bolt that has a hole drilled through it's shaft;
- this would be a new part number. We used to do an insert -> Part Copy in Solid Edge, but PDM needs improvements when it comes to part->part refs so we use an assembly with cut.

2. A normally round belt that is formed into a specific shape around pulleys;
- we don't have V-belts but air hoses, wires, looms etc. In Solid Edge we didn't model them, just wasn't enough value added for the effort of maintaining it. Solidworks has Virtual components so we can model the wire, loom, hose, etc in the assembly and not bother with managing all those files.

3. A compressed O-ring;
- we don't model compressed o-rings, but we do have foam parts that are fabricated or molded per print but they conform to a different shape when assembled. We've been using configurations for this, but it's not without compromises.

4. A PCB board that has it's edge trimmed to fit in a very tight space;
- if this is a process done at "final assembly" then it would be a cut operation in that assembly. If it's inventoried after trimmed then it's a new part number and new file.

5. A Li-Po battery with wires and connector sticking out of it, and these wires are bent into a specific location;
- these suck. For us there is not enough value added to deal with the file management and maintenance.

6. A threaded rod that has been trimmed in length;
- new part number.


+++A little story about Item #2. Some rather new Engineer was working on a new project a couple years ago and modeled up the various shapes of hoses, wires and looms in the part files that carried the purchased part number for a roll of the item. I didn't realize how it was done at the time and they left the 3D sketches of the configs of the wire, loom, etc in the part file referencing other parts in the various where used assemblies.

Several months ago ECR came through to simply replace the 6mm loom with 3/8" loom. Explain to me how to do this. I cannot copy the config from the 6mm loom file to the 3/8" loom file. simply changing the diameter of the loom in the file from 6mm to 3/8" is hack and would have the wrong size model for the part number. Now all the fancy configs in the various part files are a maintenance nightmare. Any simple change in which loom, wire or hose in any of the kits that use them requires completely remodeling all the shapes of that component in the other file. This is why we didn't model them in the past with SE. Now we are considering using virtual components in the where used assembly.