Modify part file, when inserted in assembly, just like the bolts in the Design librar

Hello Colleagues,


I am starting this thread, as I have not found any related threads here on a problem with SolidWorks, that I really am to solve.

I try to create a pipe, that has three parameters: outer diameter (D), wall thickness (T) and length (L).

When I insert the part in an assembly I want to have a drop-down menu to choose a standard D and T, plus an extrude tool to vary the L according to my technical needs in the drawing, but L should not exceed a certain manufacturing length.

The bolts from the Design Library have exactly the properties, I ask about here.

I tried to create a pipe in a part file and configured it at the standard sizes. When I inserted it in a part file and modify the extrusion, the extrusion is inevitably saved in the part file.

Is there a way to create a part file, that I can modify by insertion without modifying the original source file, like the bolts from the Design Library?

Thank you for regarding my question.


Kind regards.

Have you tried using design tables?
Yo can also go even higher and use global variables with external excel files.

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Originally Posted by Jeffrey Meyer

Have you tried using design tables?
Yo can also go even higher and use global variables with external excel files.

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Thank you for Your reply, Mr. Meyer


I have not tried design tables for a good reason. Normally one needs pipes on different variety of lengths and I cannot consider it plausible to have separate configuration for every possible size, that will eventually be needed.

The pipes are usually manufactured at size of 6000 mm and this theoretically means 6000 different configurations for each combination of diameter and wall thickness in a long term.

I will be glad to hear more about Your second idea, if it is not about creating a multitude of configurations in a single part file.


Regards.

Have you looked at weldments? With those you select the diameter and wall thickness from a list and a sketched line in your model serves as the centerline of the tube and determines its length. The lines can be curved or straight. These are more correctly tubes and not pipes but you can create your own standard sizes and make them anything you want (or anything you can buy).

Hey Bill, do you ever miss Cadkey where you could model anything explicitly, without creating a separate file and sketch for every single component? No constraints... :P

Nope. :D You can ignore a lot of what SWx brings and create dumb(er) solids but I don't see any reason to do that. I like being able to create similar parts editing a few dimensions instead of starting over.

All the years I spent using CadKey and can't even model a box in that software anymore..........

Quote:

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Originally Posted by cwilliamrose

Have you looked at weldments? With those you select the diameter and wall thickness from a list and a sketched line in your model serves as the centerline of the tube and determines its length. The lines can be curved or straight. These are more correctly tubes and not pipes but you can create your own standard sizes and make them anything you want (or anything you can buy).

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Thank you for Your reply.

I tried this, but as far as I can understand you and implement it, I don't see any difference between Your suggestion and the sweep/extrude tool.

I still have to save the part back form the assembly.

This is not my goal, but I would rather control the length of the tube (as You rectified me) within the assembly file, without modifying the source part file. Also the tube part file must be used in more than 1 assembly and all of the assemblies could have different value for the length of the tube. EDIT: Just like the bolts from the Design Library. Everybody knows the bolts from the Design Library, right?

If Your reply is exactly achieving this, probably I have to ask You to be more specific and comprehensive, since I cannot arrive to my goal with that much explanation.

Best regards.

Quote:

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Originally Posted by cwilliamrose

Have you looked at weldments? With those you select the diameter and wall thickness from a list and a sketched line in your model serves as the centerline of the tube and determines its length. The lines can be curved or straight. These are more correctly tubes and not pipes but you can create your own standard sizes and make them anything you want (or anything you can buy).

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Thanks for Your reply.

Probably You could suggest some solution to my problem?

Best regards.

The bolts and other hardware items in the design library have all the configurations for the available sizes already created. The files for these parts can get quite large depending on how many configurations exist. They are very handy because any size is there ready to be selected.

The toolbox has similar functionality with the major difference being the sizes available for a given fastener are not in the part file as a configuration until that size is used for the first time. It keeps the part file size smaller biut you need to use the browser to call up a new size and have its configuration created. The toolbox has its own overhead so it's not a free ride. If you work in the PDM environment everyone has to share the same toolbox which can be a real PITA if you are a remote user.

Weldments are a different animal. If you're modeling a structure the members of the structure exist in a single the part file as separate bodies. They are easier to deal with because the weldment function does the tedious stuff for you, all you need to do is lay out the structure as lines in 3D space. When creating a new structural member you select the type and size of that member (example: 3/4" OD x .035" wall round tube) and the line in your layout where that member will reside. A plane is created on one end of the selected line and a sketch inserted for the tube size, the tube is then extruded along the line selected. The various tubes can be trimmed to fit adjacent members -- again with the software doing the tedious stuff for you. You end up with a cut list of the various bodies you have created but you don't have a part file with configurations for the various sizes and lengths you have used in the models you're creating. This may not be what you need which was why I asked if you had looked into the weldment function. The advantage of these multi-body parts is that you should be able to edit the lengths from within the assembly. I have not tried using the weldments in this way and it may not suit your needs.

Quote:

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Originally Posted by cwilliamrose

The bolts and other hardware items in the design library have all the configurations for the available sizes already created. The files for these part can get quite large depending on how many configurations exist. They are very handy because any size is there ready to be selected.

The toolbox has similar functionality with the major difference being the sizes available for a given fastener are not in the part file as a configuration until that size is used for the first time. It keeps the part file size smaller biut you need to use the browser to call up a new size and have its configuration created. The toolbox has its own overhead so it's not a free ride. If you work in the PDM environment everyone has to share the same toolbox which can be a real PITA if you are a remote user.

Weldments are a different animal. If you're modeling a structure the members of the structure exist in a single the part file as separate bodies. They are easier to deal with because the weldment function does the tedious stuff for you, all you need to do is lay out the structure as lines in 3D space. When creating a new structural member you select the type and size of that member (example: 3/4" OD x .035" wall round tube) and the line in your layout where that member will reside. A plane is created on one end of the selected line and a sketch inserted for the tube size, the tube is then extruded along the line selected. The various tubes can be trimmed to fit adjacent members -- again with the software doing the tedious stuff for you. You end up with a cut list of the various bodies you have created but you don't have a part file with configurations for the various sizes and lengths you have used in the models you're creating. This may not be what you need which was why I asked if you had looked into the weldment function. The advantage of these multi-body parts is that you should be able to edit the lengths from within the assembly. I have not tried using the weldments in this way and it may not suit your needs.

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Weldments will this be then. Thank You for Your help.