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Adjustable Parts in Assemblies

Question asked by Bruno Protz on Apr 22, 2009
Latest reply on Feb 6, 2015 by Raul Borobio

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Hello,

I wonder if there is any method to make the parts that created adjustable? For example, I have a part of 3 meters as in the example below and want it to automatically adjust to get near a wall or another piece.

LINK TO IMAGE

How to do my part adjustable without losing your name?

Thanks

Bruno

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Don Vanzile Apr 22, 2009 2:28 PM
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Search the help file for assemblies, mates, and move component, to start.

Don
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- Bruno Protz @ Don Vanzile on Apr 23, 2009 2:11 AM
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  Seriously, I could not do this find this kind of config in Solidworks, Solid Edge is the very easy to do this kind of configuration on my part, but I can not find anything in Solidworks, sorry, I am a new user and have not have much dexterity with the software, many things seem hinder for access by the user. The software is very good, but needs time for users to adapt to it.
  
  Thanks
  Bruno...
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  - Don Vanzile @ Bruno Protz on Apr 23, 2009 10:00 AM
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    Not sure I understood your question now, do you want to make the lengths get longer and shorter and add the cross feature pattern as well?
    
    Either way, this is very easy in solidworks if you know the right tools. I would go through a few tutorials in the help menu and you should be up to speed in no time.
    
    Don
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  - John Burrill @ Bruno Protz on Apr 24, 2009 3:38 PM
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    OK, bruno, I think I understand what you're trying to do.
    You want to be able to install the blue section of conveyor and adjust it's length so that it fits between th t-junction and the other section of conveyor.
    The big thing you have to resolve first is your assembly structure.
    1) Is the entire conveyor system a single assembly or is each section a subassembly
    2) Are the odd sections going to be created by chopping a standard section or are they giong to be custom fabricated.
    the frame is a single assembly, I'd look at using a layout sketch to define the complete run of the rails (layout sketches are in the online help and where the splits occur
    If your assembling standard conveyor sections and chopping them during installation to make the odd sections, I'd use assembly cuts to trim your blue conveyor to the edge of the junction (if the junction moves, the conveyor will update)
    if you're custom fabricating the odd sections, I'd lay out your standard sections, create new subassemblies for the odd sections and use the extrude upto body end conditions to set your rail lengths and then add in your rollers and splice plates. IF you want to round your lengths to standard sizes, you can use equations to do that.
    Topics to read up on in the on-line help:
    incontext references
    assembly features
    layout sketches
    extrude end conditions
    top-down modeling
    Good luck.
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Alan Stoldt Apr 23, 2009 10:55 AM
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Bruno Protz wrote:

Hello,

I wonder if there is any method to make the parts that created adjustable? For example, I have a part of 3 meters as in the example below and want it to automatically adjust to get near a wall or another piece.

LINK TO IMAGE

How to do my part adjustable without losing your name?

Thanks

Bruno

Bruno,

Welcome to the forums.

Again, I am not clear on what you are trying to achieve, even looking at the photo.

Solid works has the ability to Parametrically drive an Assembly. A conveyor could be longer or shorter and have different numbers of rollers depending on the length.

Below is an example with Bearing Rails and a Base Plate:

This is done using Layout Sketches, Equations and a Design Table

Hope this helps to pint you in the right direction.
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Raul Borobio Feb 5, 2015 3:45 AM
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Hello

I also was a Solid Edge User and was trying to make an adjustable part.

With SE you can design a part (like an extruded profile) and set the lenght variable (L) as a driven variable for making the part adjustable.

By this way, in an assembly you can dimension a distance between two faces, set that dimension as variable and then, insert de adjustable part. The software asks you the assy variable you want to equal to the 'L' (Lenght) variable of the adjustable part.

The advantaje of this method is that you only need to have one part for all of your assemblies. No needed to duplicate parts for new assemblies.

Is there a way to work like this way in SW?
I hope I've explained correctly. Sorry but my english is a bit poor.

Thank you.
Regards
Raúl
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- Deepak Gupta @ Raul Borobio on Feb 5, 2015 4:14 AM
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  You can create configurations in the part file with predefined lengths OR use configuration publisher to define the length as required in assembly and then configurations will be automatically build.
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  - Raul Borobio @ Deepak Gupta on Feb 5, 2015 4:25 AM
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    Thanks Deepak
    
    It seems that's not possible then...
    
    Thank you
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    - Deepak Gupta @ Raul Borobio on Feb 5, 2015 4:45 AM
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      I didn't say it is not possible but I suggested you a different method than SE.
      The advantage of this method is that you only need to have one part for all of your assemblies. No needed to duplicate parts for new assemblies.
      And I'm not convinced that you can use same part with varying length for each assembly. How do you specify the length in the component drawing then? Plus i'm sure they must be auto creating configurations inside.
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      - Raul Borobio @ Deepak Gupta on Feb 5, 2015 5:50 AM
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        No, the adjustable part has a length of for example 100 mm. When you insert the part in an assembly you can chosse between adjustable or rigid part.
        If you choose rigid part, your part will have 100 mm of length. If you choose adjustable, SE will ask you for choosing the assembly variable you want to equal the length. You can do this to all assemblies you need and the original part still unmodified. It's like a 'virtual' part. The inconvenient is that you can't draw a drawing of this part. I allways use it for extruded profiles.
        
        Thank you Deepak.
        
        Regards.
        Raúl
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        Deepak Gupta @ Raul Borobio on Feb 5, 2015 5:59 AM
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        Not sure this would work but you can create a virtual part and define the extrude by up to surface option for both directions. And then in assembly choose the required two faces. Save the part externally in library and when you insert it into any assembly, change it to save internally.
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        Raul Borobio @ Deepak Gupta on Feb 5, 2015 6:09 AM
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        OK, I'll try.
        Thank you Deepak.
        
        Regards
        Raúl
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        Mark Kaiser @ Raul Borobio on Feb 5, 2015 10:07 AM
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        Here are two posts with example files for top-down assembly design methods, will take you some time to go through and understand probably, but are great examples. Old files, hoping they still open good in newer versions of SW.
        
        https://forum.solidworks.com/message/247837#247837
        
        https://forum.solidworks.com/message/14544#14544
        
        Follows John's excellent advice above.
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        Raul Borobio @ Mark Kaiser on Feb 6, 2015 12:45 AM
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        Hello Mark. I know the tp-down assembly design method. I've been working like this for a long time in SE and I'm making some complex models now with SW. The question was about to create an adjustable part like I did in SE.
        If it's not possible I'll design it with a simple line sketch to be followed by a predefined library profile.
        
        Thank you.
        
        Regards.
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