Design approach help

Discussion in 'SolidWorks' started by Martin, Feb 6, 2005.

  1. Martin

    Martin Guest

    I need to design a solid model for an elastomeric keypad. With most of the
    2D design work now done in AutoCAD it is time to move it to SW. I am
    looking for recommendations as far as the best approach to attack this.
    Here are some areas of concern:

    First, I've had trouble trying to import even single DXF layers into SW as
    the basis for a sketch. Within ACAD each button type is a multi-layer
    block. I only need one of the layers for SW sketch purposes. The touble is
    that SW only seems to want to bring in one of the instances of each blocks
    rather than the whole 50-some button keypad at once. I've resorted to
    turning off all layers except for the one I want prior to saving a DXF, to
    no avail. Next I'll try to explode all entities before DXF output to see
    what happens. Any recommendations on this front?

    The design has about fifty buttons of four different types. Ideally, I
    would create solid models of the five buttons and then bring as many as I
    need of each into an assembly. There are two possible variables:

    (1) The height of the buttons is dependant on the thickness of the panel
    that they will protrude through. This is not yet known but assumed to be
    0.125in. at the moment. This may very well be half that by the time it is
    actually made.

    How do I create a part and/or assembly that can take the panel thickess as a
    parameter for extruding the buttons? The formula would be something like
    "height = panel_thickenss + button_protrusion". The "button_protrusion"
    parameter will be different for various buttons and might range from 0.000in
    to 0.100in.

    (2) Each button will have a different legend or graphic laser cut onto the

    How do I design a part that I can then replicate many times within an
    assembly yet change the legend sketch during assembly creation time?

    As I get into the assembly there are other considerations. One is that the
    buttons are joined at the bottom by a silicon rubber matt about 0.050in
    thick. The easiest way to model this is a simple 0.050in rectangular
    extrusion. However, each button has an underlying structure that cannot be
    filled in by this matt. My thinking is that the model for each button will
    be designed with a small square section of matt, enough to allow for the
    underlying structure and also to aid in mating. How do I get the button to
    cut a hole in the solid matt when placed into the overall assembly?

    Simarly, I would like to have each button cut a suitable hole in the front
    panel based on a given clearance, say 0.010in. What's the best way to
    approach this?

    I've been reading a lot on the archives about issues with incontext mates
    and related assembly matters. As a new user (about two months) some of this
    is confusing/daunting in that there's great fear of making assemblies that
    self-destruct (I've already had that happen). The worst of it is not
    knowing whether it is a "free SW feature" or an aspect of the approach taken
    in building either the parts or the assembly. I've taken the one-week "SW
    Essentials" course and will probably follow-up with the Advanced version
    after I get about six months' experience. For now, I could use a shove in
    the right direction.


    Martin, Feb 6, 2005
  2. Martin,

    I have a reccomendation,,,,,, STOP !!!!!!!!!!!!! back away from the
    computer! Take a deep breath,,,,,,, ahhhh, that's better.

    First off, Solidworks doesn't work anything like ACAD. Importing sketches
    from ACAD is a mistake, and will cause you nothing but problems. It's much
    better to start from scratch in SW, and do it the SW way.

    To this end, I suggest you go through some of the online tutorials. Pay
    special attention to sketching and linear "feature" arrays (not the sketch
    array variety).

    Take two aspirin

    Call me in the mornin


    Mark Mossberg, Feb 6, 2005
  3. Martin

    matt Guest


    To me, it sounds like you have the Acad to SW order mixed up. If anything,
    you should start in SW. I'm kind of curious how you can do the 2D design
    in Acad and now get ready for more design in 3D.

    DXF layers... you can explode layers in SW if you just import the whole
    dxf, but take Mark's advice and learn to work in SW and try to forget Acad.
    There are several ways of getting Acad data into SW sketches, but none of
    them is really something I'm fond of. Be careful of the imported 2D data,
    make sure it's really what it seems. Add relations and dimensions to it to
    fully define the sketch.

    As for getting an offset cut outs around your buttons, there are lots of
    ways of doing this, but I would use intersection curve or might even try
    the new Indent function. Other possibilities include cavity, join or
    convert entities. Look the functions up in the help, and it should become
    clear to you whether it will help you get where you need or not. Most of
    these functions will depend on whether you are doing all of this in a part
    or in an assembly.

    Use equations for the variable heights, or check out global variables or
    even link values.

    It's good that you're taking training to get things figured out. Sounds
    like you want information faster than they can give it to you, though.

    Good luck,

    matt, Feb 6, 2005
  4. Martin

    jon banquer Guest

    "First off, Solidworks doesn't work anything like ACAD. Importing sketches
    from ACAD is a mistake, and will cause you nothing but problems. It's much
    better to start from scratch in SW, and do it the SW way."

    What a massive waste of time !!!!

    The SolidWorks way means you have to redraw everything from scratch because
    SolidWorks is a program that hates non-native imported geometry.

    Lets compare starting from scratch with SolidWorks to VX :

    In VX you import the Autocad wireframe (dxf or dwg) and use it ! It doesn't
    even import into the skectcher... comes right into the model / assembly

    All you do in VX is extrude the wireframe AutoCAD geometry to a solid. If
    you need to rotate a section of the wireframe geometry to do a revolve no
    problem, etc....

    Why use a program that hates non-native geometry ????

    Forget the asprin:

    Dump SolidWorks and get a program that doesn't treat non-native
    geometry like some sort of illegal alien.

    jon banquer, Feb 6, 2005
  5. Martin

    jon banquer Guest

    To me it sounds like just another case of how SolidWorks can't cope
    with real world conditions / data from other modelers.

    Why use a CAD/CAM product that is so limited in it's approach ?

    jon banquer, Feb 6, 2005
  6. Martin

    Martin Guest

    Mark Mossberg wrote;
    OK. Done.
    I've been using ACAD since version 1.2 (can you say 8in floppies and CP/M
    system?). So, I am used to using it as a thinking tool. In this particular
    case I've simply used it to play with layouts, 2D clearances and general
    ideas. Sort of like paper and pencil. Now, with that out of the way, I
    need to graduate the design to s solid model to submit to the fabricator.
    This is simple enough that starting from scratch with SW is not a problem

    I am sort of taking this as a learning opportunity as well, and so, I wanted
    to figure out if it makes sense to, at the very least, import button
    outlines (front view) via DXF/DWG. Of course, the first thing that happens
    is that the sketch comes in with no constraints or relationships whatsoever.
    With more complex sketches there would be a non-trivial amount of work in
    constraining the sketch.

    Unless I'm missing something, the simple rounded rectangles and circles for
    my particular excercise do not suffer from being imported and
    hand-constrained this way vs. being created from scratch within SW.

    To address your first statement, yes, absolutely, SW does not work anything
    like ACAD and one shouldn't even think the ACAD way when using it. I'm
    progressively getting better at this and the questions I asked (and those
    that I will undoubtedly ask in the near future) are a reflection of the fact
    that I am trying to better understand how to do it the SW way.
    I'll lookup feature arrays. Not sure I remember that. I've done all the
    online tutorials as well as going to the class and going through most of the
    sheetmetal coursebook. Now I have information overload. The new mission is
    about connecting the dots and making it work under fire without taking

    Thanks for the pointers,

    Martin, Feb 6, 2005
  7. Martin

    matt Guest

    Don't hand constrain all the unconstrained imported Acad data. Use Tools,
    Relations, Constrain All. This will only work if there are no relations in
    the sketch. It may be advantageous to delete any existing relations, and
    use this to recreate them all automatically.
    matt, Feb 6, 2005
  8. Martin

    Martin Guest

    See my prior post regarding this. It's about being a nearly 20-year ACAD
    user two months into a new tool. I can run ACAD without thinking about the
    mechanics of the program. As is evidenced by my questions, I'm not there
    yet with SW (only a couple of months on it) and so, it is much easier for me
    to doodle in ACAD than in SW.

    BTW, I've read through most of your site. Thanks for taking the time to
    post such useful material.
    I'll look these up. I'm looking for the solution that will have the
    assembly and related parts automatically adjust to design changes. For
    example, if my vendor tells me that the buttons need to be 0.010in wider, I
    want the holes cut in bezel to change when I change the part and do so
    according to the clearance rule I specified.

    I just have to get work done. I can't be in learn-and-no-work mode forever.
    I'm willing to accept making mistakes as I go. Make enough of them and you
    become an expert! :)

    One of the problems with the SW training (all manufacturer training, for
    that matter) is that the folks who teach are not always accomplished
    practitioners. Sometimes they are not even good teachers. I've seen the
    worst and the best. The SW class I took was good, but not the best by a
    longshot. The material is there, in the book, but the instructor would have
    been better positioned in front of a kindergarden class.

    That's real life, I guess.

    Thanks again,

    Martin, Feb 6, 2005
  9. Martin

    Martin Guest


    While I appreciate your comments, I don't --and I say this with the utmost
    respect-- have any use for them. Engineers have to learn to live in a
    non-idea world. If I had it my way, I'd be off on a dive boat in the
    Caribean and someone else would be duking it out with whatever CAD system to
    get this design done over a weekend.

    When I first started to use ACAD nearly twenty years ago you had to load and
    unload modules from memory; convert DWG's to DXF and edit them with WordStar
    just to get the damn thing to be usable for real-world designs. We made it
    work and it served its purpose. Now, for me, it's about adding a new tool
    to the arsenal: SW. It matters not that it might be the best or the worst
    out there, it's what I have to work with.

    By all means, if you have anything to contribute that could help understand
    (me and others) how to approach SW at my level I'll humbly listen and learn.


    Martin, Feb 6, 2005
  10. Martin

    Martin Guest

    The sketch where I tested this is a simple rounded rectangle. 0.210in to
    the side and 0.03125in radiuses on all corners.

    I displayed all relations and deleted all my hand-applied relations.
    Then I used the "Constrain All" function.

    This just added tangent, vertical and horizontal relations. The sketch
    remained under-defined. In order to fully define it I still have to add
    dimensions and a relationship to the origin.

    Which brings-up another question:

    To fully define the sketch dimensions and additional relations are needed:

    - The you dimension one arc and tell the other arcs that they are equal to
    the first.

    - Horizontal and vertical relations from one vertical and one horizontal
    side to the origin.

    When it comes to the sides, you can dimension this sketch three ways (maybe

    1- Length of each linear segment
    2- Inside distance from side to side
    3- Inside distance from the intersection of an arc and a line to the same
    point on the opposite side

    My gut feeling is that [2] might be the most appropriate (whatever that
    means) way of doing this. Correct?

    Martin, Feb 6, 2005
  11. Martin

    jon banquer Guest

    Understand that driving SolidWorks can be like showing up for Indy 500
    on a moped and expecting to be competitive. It doesn't matter how good
    you are, without the right tool sometimes one can't be productive.

    The FACT is that what SolidWorks makes you go through by having to
    start all over again by drawing everything from scratch is an insane

    VX can easily work with imported wireframe. SolidWorks can't.
    Start asking yourself why SolidWorks should not be able to work
    with imported wireframe. Does this severe limitation of SolidWorks
    make ANY sense ??? How can this limitation be justified ???
    Throw SolidWorks in the garbage and get a real CAD/CAM tool.

    Or :

    Stop accepting the massive limitations of SolidWorks and demand more
    from a CAD/CAM product. This is a typical real world problem that
    SolidWorks falls apart on.

    VX handles this kind of thing with ease.

    jon banquer, Feb 6, 2005
  12. Martin

    Martin Guest

    I apologize for my ignorance, what's "VX"?

    Martin, Feb 6, 2005
  13. Martin

    troll Guest

    <snirk, sniffle>
    Esk im for the drawin and sho im how good it wurks jon. Then yu kin stert
    tha secund thred on the new VX forum. Or maybe yu already been banned.
    troll, Feb 6, 2005
  14. Martin

    jon banquer Guest


    Take a good look at the videos posted showing how VX works with imported
    wireframe data and easily turns that imported wireframe data into a
    parametric solid.

    It's very important to understand what SolidWorks should be able to do but

    Take it another step and download VX and try doing it yourself. VX makes
    it very easy.

    jon banquer, Feb 6, 2005
  15. Martin

    Cliff Guest

    That clueless wants to hump your leg <G>
    Cliff, Feb 6, 2005
  16. Martin

    Cliff Guest

    It's the buzzword of the day.

    Cliff, Feb 6, 2005
  17. Martin

    Cliff Guest

    You don't use ANY CAD system at all, clueless.
    Probably never have.

    Still driving a truck?
    "Parametric" way over your pointed little head?
    "History" as well?
    Cliff, Feb 6, 2005
  18. Martin

    Cliff Guest

    Clueless idiot.
    Cliff, Feb 6, 2005
  19. Martin

    Cliff Guest

    XAS, etc. importing, huh?

    Your wisdom on & knowledge of these subjects is just astounding,
    as usual.
    Cliff, Feb 6, 2005
  20. Martin

    Bo Guest

    I have done some of these sorts of things and some other experienced
    SWks users are on track.

    It sounds like you have not really gone through the SWks Tutorial or
    taken an introductory class that covers that material as a first step.
    Once you go through those basic operations in the tutorial, which was
    maybe 80 pages when I did it, you will get your mindset for how
    SolidWorks functions for basic things. That is essential, but easy.

    The logic of certain design methods will start to become apparent as
    you start designing with draft, versus adding draft later, and there is
    no "Right" way to do this. The nature of the part and the way the
    tooling HAS to be built often determines which way is best or required.

    Other construction details can likewise be done several ways, and this
    initial openminded experiment and learning phase of a few days to a
    week will set you in good stead for quickly determining the methods to
    try in your project.

    For me, I must admit, I sometimes make 3-4 designs of a particularly
    complicated part, with sometimes 2 different initial starting points.

    Some parts just have no chance of parallel walls, so "Shell" doesn't
    work, or can work only in a limited area, which gets drawn first or
    drawn as a separate solid and shelled and then connected to the rest of
    the part design. I've actually cut out a part of a solid as a separate
    piece to accomplish this once.

    Some part constructions are totally determinined by the need for
    specific locations of parting lines, so that I can't just "Loft a cut"
    through an area where 2 cores split.

    In the "old days" this sort of expertise was called "having time on the
    board", meaning the drafting table. Now its similar in "screentime in
    Solidworks". Shouldn't take you too long to fly.

    Bo, Feb 6, 2005
Ask a Question

Want to reply to this thread or ask your own question?

You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.