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Solidworks, auto fit V slot

Discussion in 'CAD' started by Adam Filipowicz, Oct 29, 2015.

  1. Adam Filipowicz

    Adam Filipowicz Veteran
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    Im new to Solidworks. still working through tutorials.

    I would like to be able to insert two corner components and then say fille the space between them with a vslot extrusion. and have its length automatically adjust. So i dont have to make a new part each time i need to make a slighly adjustment.

    anyone know how to accomplish this?
     
  2. Joe Santarsiero

    Joe Santarsiero OB addict
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    Do you want the corners to adjust with it?
    There are a few ways to do it. For your use I might create the vslot using extrude midplane.
    Create an assembly.
    Attach the corner components to the extrusion in the assembly using mates.

    Now you just edit the length value of the extrusion.

    Joe
     
  3. Adam Filipowicz

    Adam Filipowicz Veteran
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    If I move the corner, i want it to adjust
     
  4. Joe Santarsiero

    Joe Santarsiero OB addict
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    There are ways to move components of an assembly and have other components feature properties change (such as length).
    For instance, two brackets that are constrained in two dimensions, but can be slid apart from each other, which in turn causes an extruded beam to change lengths.
     
  5. Adam Filipowicz

    Adam Filipowicz Veteran
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    Sounds good.. now how to I set that up lol
     
  6. Joe Santarsiero

    Joe Santarsiero OB addict
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    Using symmetry method.
    New assembly
    Insert beam
    select the beams extrude feature and edit it to extrude midplane.
    Insert two brackets.
    Using mates, you must constrain the brackets to the beam so they slide along the beam in position. This is difficult to write steps to so you will have to hash it out. Shouldn't be a problem.
    Once you have the brackets sliding up and down (and off of) the extrusion you will want to create a symetric relationship between the two by using mates:
    Selecting mates, symmetry mate, select opposing faces of the brackets, as your symmetry plane you will select the central plane of your beam (extrusion plane) or the central plane of the assembly that is coincident with the beams extrusion plane.
    Now, you should be able to grab one bracket and slide it along the beam as before. the other bracket will mirror its position on the other side of the beam.
    Next, to make the beam flexible:
    Select and edit the beams extrusion again.
    under direction 1 choose extrude up to surface.
    Select a surface of the bracket in that direction.
    Check the direction 2 box.
    Select extrude up to surface.
    Select a surface of the opposing bracket.
    Green check mark out.

    Now you should be able to grab the brackets and pull them apart or push them in. The length of the beam extrusion will change accordingly. If it doesn't change immeadiatly then hit the rebuild icon at the top of the screen (looks like a traffic light).

    Joe
     
  7. Adam Filipowicz

    Adam Filipowicz Veteran
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    Thanks Joe. it took some messing with but I got it working!. your an amazing person! :)
     
  8. Adam Filipowicz

    Adam Filipowicz Veteran
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    everything was working well until i tried to rotate and then everything started to seperate and then i hit rebuild half of the components disappeared :), bunch of error messages
     
  9. Joe Santarsiero

    Joe Santarsiero OB addict
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    What did you try to rotate?
    This may not be the best method for what you're trying to do. Sometimes a fixed end of the beam is required.
    Extrude the beam in one direction.
    Attach brackets as before.
    Create a reference geometry plane at the center of the beam by referencing both ends.
    Add symmetry mate just as before and so on.
    This should create a beam that doesn't mind being fixed at one end while dragged at the other.

    All in all, Solidworks doesn't like working this way. Use of design tables and configurations are handy to know.
    A completely drag and size machine is tricky to do without having Solidworks puke all over itself. Evaluate/measure and undo(when it works!) are your best friends.

    Joe
     
  10. Jestah

    Jestah Veteran
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    for building Vslot frames I often use the weldment feature based from a 3d sketch as then you can keep a lot of the build within a single sketch. I like this method as within this function you can offset different sticks from each other by a set value to create clearances as well as get a detailed cut list of all the required sticks.

    It requires a bit of setup to create the profiles within your library but once done building up complex frames is fast and ready for you to then drop your hardware onto.

    A video for showing the basics
     
  11. Adam Filipowicz

    Adam Filipowicz Veteran
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    Thank you very much. thats very helpful
     
  12. Joe Santarsiero

    Joe Santarsiero OB addict
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    Weldment is another way to build. It doesn't offer the drag and size that you were looking for. I use weldments quite a bit at work. Solidworks doesn't come prestocked with everything so you will have to save some custom profiles into a weldment folder. Fairly easy thing to do.
     
  13. Jestah

    Jestah Veteran
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    Surely dragging out the lines in the 3d sketch to give you the same effect? I always find how other people model really interesting and keen to know the limitations of a feature or method as I am somewhat self taught and understand there are millions ways to fillet a cat ...
     
  14. Joe Santarsiero

    Joe Santarsiero OB addict
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    You can drag the sketch around but you can't see the profile you are dragging in relation to other parts. Not a huge deal, but in Adams initial post it sounded like he wanted the brackets to control the length of the extrusion. Editing the weldment sketch would be the other way around. There's definitely a number of different ways to do things though.
     

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