Hose Assemblies

[Tapani Sjöman]

I'm building a Grease Piping System with multiple hose assemblies in it. I have for example 4 identical, 400 mm long hose assemblies with 90° elbow in another end. I have made these assemblies virtual and I use external links to get second end to the right position.

Is there a better way to make this? How do you make this kind of task? Maybe save hose assembly as a part and make it more simple that way?

[AlexLachance]

That is pretty much how we proceed for hoses. I think having it any other way would lead to a load of hassle in file management.

[bnemec]

We would do similar, except no external refs to other parts through the assembly.

Also, because of how PDM and how SW Virtual Components behave we're using them less and less. Nothing catastrophic but enough to make it simpler to just use real files.

[Tapani Sjöman]

Thanks for quick replys! Hose assemblies are bit complicated, while need to keep these flexible. If not virtual parts, then need to save each hose assembly with a unik name to keep them flex. And can't use them in another assemblies either. Hmm.

[bnemec]

You are correct they can become complicated quickly. Not so much from CAD itself, but all the external "things" we have to accommodate.

We have a fresh example of a 12v air compressor kit that has hoses, wires, switch-valve and corrugated loom. Everything we work with has part numbers, 14ga orange wire, black wire, the various hoses and various sizes of looms each have a purchased part number. In our case the product support group is now remodeling several kits just to change on section of loom to another size. Each pc has a shape for how it's used in final assembly and a simpler shape for making up the kit. Those shapes were modeled up as configurations in a file for that specific hose or wire or loom. We're not going to just change the loom diameter in one configuration because the file represents a specific purchased part number; cannot have different sizes in that file. There is no way to copy a configuration from one file to another (copy the existing loom model from the 6mm loom file to the 10mm loom file for example). Because changes like this are common for us we do not model wire, hose, loom, etc in a file for the purchased part (a model of that should be a spool or drum) Instead they get their own file. Strangely some of those models may wind up with multiple where used due to several kits that are nearly the same but a just a little different. Naming the files is not a problem, we use PDM serial number for file names.

Enough about what we do, if you're not using PDM and want to make sure the hose model doesn't get used elsewhere then I think a virtual component will work well.
There was something about VCs in Pack and Gos but I cannot remember if that was an old issue and only in special cases.

[berg_lauritz]

You are correct they can become complicated quickly. Not so much from CAD itself, but all the external "things" we have to accommodate.

We have a fresh example of a 12v air compressor kit that has hoses, wires, switch-valve and corrugated loom. Everything we work with has part numbers, 14ga orange wire, black wire, the various hoses and various sizes of looms each have a purchased part number. In our case the product support group is now remodeling several kits just to change on section of loom to another size. Each pc has a shape for how it's used in final assembly and a simpler shape for making up the kit. Those shapes were modeled up as configurations in a file for that specific hose or wire or loom. We're not going to just change the loom diameter in one configuration because the file represents a specific purchased part number; cannot have different sizes in that file. There is no way to copy a configuration from one file to another (copy the existing loom model from the 6mm loom file to the 10mm loom file for example). Because changes like this are common for us we do not model wire, hose, loom, etc in a file for the purchased part (a model of that should be a spool or drum) Instead they get their own file. Strangely some of those models may wind up with multiple where used due to several kits that are nearly the same but a just a little different. Naming the files is not a problem, we use PDM serial number for file names.

Enough about what we do, if you're not using PDM and want to make sure the hose model doesn't get used elsewhere then I think a virtual component will work well.
There was something about VCs in Pack and Gos but I cannot remember if that was an old issue and only in special cases.

Apart from PDM (which sucks with virtual components) virtual components have several downsides to them that should never be overlooked, here are some issues I have experienced in the past with them:

• If the component with the virtual components inside it becomes corrupt - all your virtual components will be corrupt as well/will be lost (Virtual components only live inside the assembly they are created in!)
• sometimes virtual components will give you weird errors like "the file at [temp location] does not match the ID" or something similar - usually happens when you first load them in large design review/lightweight and then resolve them
• Virtual components in general suck BIG TIME(!!!!!) for performance: SolidWorks needs to resolve the assembly & the virtual component when loading resolved (example: We changed our roof assemblies from mostly virtual parts to all part numbers - the load time of the assembly (the drawing was even worse!) decreased by over 30% resolved!])
• The performance impact is even greater when you have nested virtual components (i.e. Virtual assembly with virtual parts in it) - also: PDM will always show an edited but not saved pencil if you have a virtual assembly with virtual parts within an assembly!

  

• It won't save them to the latest version if you do not resolve them if you upgrade SolidWorks

After having to work on a large scale with virtual parts I started to despise them for manufacturing production drawings/models.
They are amazing for prototypes/smaller assemblies etc. though.

Edit:
Most of the virtual components we work with are simple "cut parts" (i.e. hoses, wires, etc.). We assign the material (wire 123-456, hose 234-345) to them and give them a part #. Our material library is extensive though and we constantly add new materials. That is why the search tool (link) is so golden for our case.

Edit: added link, picture and removed the lightweight statement. That is not true, it was only perception it seems. Maybe it's only when saving drawings lightweight? I'm unsure now.

[Frederick_Law]

SW create temp file for each virtual component. Not sure how PDM handle that since temp file will be deleted.

[berg_lauritz]

SW create temp file for each virtual component. Not sure how PDM handle that since temp file will be deleted.

same!

[DanPihlaja]

I create 1 part, make it a weldment, drop it into the assembly, then edit it in context and add all the hoses as bodies to that 1 part using in context relations to the components that they attach to.

Then, I can reference that 1 part and get lengths of each hose in the weldment cutlist.

Then I make that part suppressed for the default configuration of the assembly and create a separate "with hoses & tubing" config to show that if needed.

This is so that the resources are being hogged unless they are needed.

[Frederick_Law]

Can you make configs of the same "hose kit" for each location?
All assemblies will ref same file with same part number and description.
There will be 1000s of configs.

[jcapriotti]

SW create temp file for each virtual component. Not sure how PDM handle that since temp file will be deleted.

PDM creates a "record" for it so it shows in the BOM but there isn't a file created since SolidWorks stores them in a temp folder. We use virtual components quite a bit for wiring and for imported commercial parts. The early years was fairly buggy but its stabilized a bit. I can't imagine not having it now, especially when we import an assembly with hundreds of components. I don't want to create part numbers for them when the assembly is the only thing we assign a number to.

[bnemec]

PDM creates a "record" for it so it shows in the BOM but there isn't a file created since SolidWorks stores them in a temp folder. We use virtual components quite a bit for wiring and for imported commercial parts. The early years was fairly buggy but its stabilized a bit. I can't imagine not having it now, especially when we import an assembly with hundreds of components. I don't want to create part numbers for them when the assembly is the only thing we assign a number to.

Our usage of VCs boil down to what Jason said ^. Design Engineering isn't really in charge of how part numbers are assigned and BOM structure. So we have some things that need a model but do not get a part number (in ERP). It's rare but it happens, in those cases the part file and the assembly files have the same part numbers. Example is a plywood board that is CNC cut then T-nuts are pressed in. The DXF for the board comes from the part file but the nuts are added in the assembly and the print uses the assembly. This is where we use VCs for the plywood part.

PDM seems to handle VCs ok when everything is working as it should, it's nut not very robust/fault tolerant. SW saves/extracts the VCs from the assembly file into a folder in your user profile and packs them back up when the assembly file is saved. If SW crashes or hangs or the save operation fails, you're kinda hosed and have to start fixing things yourself. Now if the user is oblivious and tries to check in the assembly later it can start getting messed up because the folder I mentioned is named after the Procsess ID of the SW session that created it. It's fixable but gets tough.

The more common workflow that we haven't figured out how to deal with in PDM is when the part goes from real to VC or VC to real. This is due to change in MFG BOMs in ERP and is rather common. Problem is if the real file has been released users do not have permission to delete it. SW doesn't offer a good PDM integration here IMO so when the user follows the SW tutorial/triaing and "Simply right click the part and select make virtual" we wind up with a single part represented in a real file >AND< also as a VC. Now if the user is oblivious again we wind up with that real file getting used in other assemblies maybe being revised, all sorts of things. If all your users completely understand PDM, or if you have a small group of CAD users and very few constraints on how you use CAD it could be managed.