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Pipes with variable lengths

Question asked by Giuliano Iodice on Sep 4, 2020
Latest reply on Sep 5, 2020 by M. B.

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Hello everyone, I ask for guidance because I'm going crazy.

I have an article (part) called "DN100 TUBE" with a fixed external circular section of 114.30 mm and a commercial length of 6000 mm (extrusion function).

I have to insert it in different assemblies and even several times within the same assembly, but each instance must have a different length, always variable, NOT STANDARDIZABLE, and above all independent from the part and from all the other instances.

What is the best way to achieve this?

Thanks in advance for your attention.

Rob Edwards Sep 4, 2020 5:39 AM

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Hi Giuliano

Infinitely variable lengths are what I have to deal with in woodwork.

In our case we do not have pdm (of which I have zero experience) and the parts live in the project folder and are not shared across projects.

I make a configuration for each use case - ie the configuration is not linked to any particular length but to where it is used.

Here's an example of a deck we did

and a sample of the pick list

As you can see this means that you can have the same lengths in different configurations - which in our case was what I wanted, especially during the design phase. Promoting all the Parts and sorting the BOM by length was sufficient for me.

Here the part number is the configuration name, which was setup to match the sub-assembly structure, which was 2 levels deep.

Understand that we are a small company, who manufacture in-house, so we do not need or understand the requirements of more professional outfits, but maybe this helps.

I mean what else can you do?

I take it you have explored the configuration publisher. I don't use it as I prefer to use Design Tables to create my configurations en masse up front, but I think it is made for your scenario.

2019 SOLIDWORKS Help - Configuration Publisher

The help files aren't the most helpful. From my recollection there are two modes of operation.

One of them allows you to create configs on the fly, the other eases the selection of an existing configuration.

See the reply in context

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18 Replies

Krzysztof Szpakowski Sep 4, 2020 4:20 AM
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Configurations, Design Table, DriveWorkXpress
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- Giuliano Iodice @ Krzysztof Szpakowski on Sep 4, 2020 4:44 AM
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  Thanks Krzysztof for your reply.
  I had also thought about configurations, but what happens when I put the part in assembly? Whenever I have to remember to create a new configuration for that particular length? Millions of configurations! What happens if I make a mistake and overwrite a value in a configuration? What a disaster in my vault !!!
  On Design Table I have strong doubts as I have already stated that the lengths are absolutely variable and cuts of commercial lengths are not standardized.
  Maybe DriveWorkXpress is my last hope but I don't really know where it is.
  Thanks again
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  - The Merovingien @ Giuliano Iodice on Sep 4, 2020 5:34 AM
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    use a DOT (DOTPRT)
    
    create for each "tube/pipe" section, one file, you can name the file with this simple rule :
    ASM (file name)= toto
    PRT for each pipe seciton (file name) = ASM-name - Pipe xx
    
    example 1 :
    ASM = toto
    PRT-Pipe = toto - Pipe 01
    PRT-Pipe = toto - Pipe 02
    PRT-Pipe = toto - Pipe 03....
    
    example 2 :
    ASM = 12345
    PRT-Pipe = 12345 - Pipe 01
    PRT-Pipe = 12345 - Pipe 02
    PRT-Pipe = 12345 - Pipe 03....
    
    in that file the "Design table" can only drive : Material, DN (diameter), thickness, description, additionnal properties
    
    you leave the length NOT driven by the table.
    you set the "table options" to "table is the king" (not update from 3d, table is the master)
    
    that mean, the user can modify only the length, by simply clicking on it.
    
    each pipe-file are independant, so if you do a special cut into one pipe file, it will only affect that assembly.
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Rob Edwards Sep 4, 2020 5:39 AM
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Hi Giuliano

Infinitely variable lengths are what I have to deal with in woodwork.
In our case we do not have pdm (of which I have zero experience) and the parts live in the project folder and are not shared across projects.
I make a configuration for each use case - ie the configuration is not linked to any particular length but to where it is used.

Here's an example of a deck we did

and a sample of the pick list
As you can see this means that you can have the same lengths in different configurations - which in our case was what I wanted, especially during the design phase. Promoting all the Parts and sorting the BOM by length was sufficient for me.
Here the part number is the configuration name, which was setup to match the sub-assembly structure, which was 2 levels deep.
Understand that we are a small company, who manufacture in-house, so we do not need or understand the requirements of more professional outfits, but maybe this helps.

I mean what else can you do?

I take it you have explored the configuration publisher. I don't use it as I prefer to use Design Tables to create my configurations en masse up front, but I think it is made for your scenario.

2019 SOLIDWORKS Help - Configuration Publisher

The help files aren't the most helpful. From my recollection there are two modes of operation.

One of them allows you to create configs on the fly, the other eases the selection of an existing configuration.
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- ömür tokman @ Rob Edwards on Sep 4, 2020 8:25 AM
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  Rob Edwards wrote:
  
  Understand that we are a small company, who manufacture in-house, so we do not need or understand the requirements of more professional outfits, but maybe this helps.
  
  Small company big jobs ..
  Hey Rob Are you not too professional for a small company?
  
  Mr humble.
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  - The Merovingien @ ömür tokman on Sep 4, 2020 8:32 AM
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    Omur, just a remark, when you "quote" someone,
    
    start what you are writing outside (after) the quote (by moving the cursor) :
    
    test toto
    bla bla bla
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The Merovingien Sep 4, 2020 5:52 AM
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"config publisher" is only to show a "friendly panel display" to the user, when he insert the PRT-configs.

he should begin simple with a "design table first"

and after, when he insert the part and if the config-list is too long for him,
then he can add the "Publisher" (publisher is an additionnal feature that require design-table)

but as it's only for pipe, the list with deisgn-table will not be too long (material, DN, thickness)
length is "indiviual to each file" and specified by the user.
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Krzysztof Szpakowski Sep 4, 2020 6:55 AM
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When I used a similar method for aluminum profiles, I used the configuration. Why? The name of the configuration included the profile type and length (making it easier for the saw operator). When this variant had a version with other features (openings, pockets, etc.), we made derived configuration. The configuration used in the "first" project was later used in other products. This meant that only one order was generated for the production. It was especially important with external partners.
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Glenn Schroeder Sep 4, 2020 7:08 AM
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One option would be to create the pipe as weldments, with a separate Part file for each instead of using configurations. By doing that you can assign a description in the .sldlfp file that will carry over to the Part as a cut list property, along with the Length, which will be automatically generated.

Another option would be to create the pipe inside the Assembly, with multiple pipes in a single Part file. (I'd still do it as a weldment). Create and edit the Parts inside the Assembly, so the end locations and lengths are driven by the Assembly. Depending on your specific needs, this might be the better option.
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Jeremiah Feist Sep 4, 2020 9:45 AM
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best way is either weldments or routing (if you have SW premium)
if you are on SW2020, the new "flexible" component may work for you here as well.
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- Giuliano Iodice @ Jeremiah Feist on Sep 4, 2020 11:29 AM
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  Hi Jeremiah
  "Flexible" component might be the right answer to this question.
  It would work like a "dynamic block" in autocad, wouldn't it?
  Thank you
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  - Jeremiah Feist @ Giuliano Iodice on Sep 4, 2020 12:20 PM
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    don't know - not an AutoCad user
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- Tom Gagnon @ Jeremiah Feist on Sep 4, 2020 1:00 PM
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  Jeremiah Feist wrote:
  
  best way is either weldments or routing (if you have SW premium)
  if you are on SW2020, the new "flexible" component may work for you here as well.
  FTFY. Routing is inferior in stability to weldments.
  
  I agree with both Glenn and Jeremiah that Weldments are the way to go. I would make it a virtual component in the assembly, but it can also be saved externally if you need to do more with it, or if it somehow also applies to another assembly. In my workflow, these virtual components use their own part template which already contains some differences relevant to me among its custom properties.
  
  If you do not find the profile you need among weldments, make your own profile and add it to among your Weldments file location.
  
  Furthermore, Weldments have drawing advantages of referencing profile description and cut length into an annotation callout. I use:
  
  $PRPWLD:"Description"
  $PRPWLD:"LENGTH" LG
  
  in a Library Note to apply to updated weldments. Note that in my scope, I do not automatically update cut lists, but rather choose to update them when producing this drawing detail. If you have small uses, automatic cut list update is not too much of a productivity sink.
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  - Giuliano Iodice @ Tom Gagnon on Sep 4, 2020 1:10 PM
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    Hi Tom
    i am currently using
    virtual components
    as workaround but
    unfortunately these
    cannot be managed
    by my pdm.
    
    Thanks a lot anyway
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  - Glenn Schroeder @ Tom Gagnon on Sep 4, 2020 1:30 PM
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    Tom Gagnon wrote:
    
    Jeremiah Feist wrote:
    
    best way is either weldments or routing (if you have SW premium)
    if you are on SW2020, the new "flexible" component may work for you here as well.
    FTFY. Routing is inferior in stability to weldments.
    
    I agree with both Glenn and Jeremiah that Weldments are the way to go. I would make it a virtual component in the assembly, but it can also be saved externally if you need to do more with it, or if it somehow also applies to another assembly. In my workflow, these virtual components use their own part template which already contains some differences relevant to me among its custom properties.
    
    If you do not find the profile you need among weldments, make your own profile and add it to among your Weldments file location.
    
    Furthermore, Weldments have drawing advantages of referencing profile description and cut length into an annotation callout. I use:
    
    $PRPWLD:"Description"
    $PRPWLD:"LENGTH" LG
    
    in a Library Note to apply to updated weldments. Note that in my scope, I do not automatically update cut lists, but rather choose to update them when producing this drawing detail. If you have small uses, automatic cut list update is not too much of a productivity sink.
    
    I have some weldment property Notes saved as Styles in my Drawing templates. That makes it much easier to insert them.
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Tim Taby Sep 4, 2020 10:44 AM
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I would use a design table. You can put custom properties in it to control the part numbers and lengths very easy. I do this with aluminum extrusions all the time. We purchase 24 ft sections of extruded material and cut them to many different lengths for many different projects. When I need a new length I just add it to the table and insert into the assembly.
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Kevin Chandler Sep 4, 2020 3:23 PM
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Hello,

Weldments are probably best due to ease, flexibility and cut props (end angles too for non-90 cuts).

A DT does have the advantage of checking lengths that would exceed stock lengths.

Kevin
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M. B. Sep 5, 2020 5:25 PM
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If you have a pipe part file with dozens or hundreds of incremental length configurations and the length of every pipe in each assembly configuration can be determined by formulas or have values entered into a stand-alone Excel file, those length values can be used with a LOOKUP or Nested IF function in the assembly design table to find the appropriate part configuration name and list it in the assembly design table column under
$CONFIGURATION@part name<1>
='path\[excel file name.xlsx]sheet name'!part configuration name
This will require some time to set-up but once completed, it will only take minutes or less to create unique new assemblies. The common values in the stand-alone file can also be used to control many different criteria involving multiple part and assembly files… Sweet!

Or, if you instead want to have a pipe part file with just one 6,000mm long default configuration, another method would use an Insert/Assembly Feature/Cut for each pipe length. The length values would come from either a stand-alone Excel file (like above) or from formulas in the assy. design table. With this method, all pipes would be “cut to length” just like what is done on the shop floor and could have any pipe length if uniform increments aren’t wanted. Assembly Feature/Cuts can be made before inserting or mating subsequent components.
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