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Thread: Toolbox - specifically smart fasteners

  1. #11
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    When you're in the McMaster site, choose the product that you want by drilling right down to the actual McMaster catalog number. At that point it will give you the option of downloading a 3D CAD file where the default file type is a native Solidworks file. You can of course use this SW file but you might find that your version of SW (student edition) may not be able to read it for one reason or another. So, instead of a SW file type download choose the STEP option - the student edition should be able to open it.
    When SW asks you if you want checking or feature recognition, answer in the negative, and give it a few seconds to build the part. Save it.

    Be aware that the McMaster STEP files produce very detailed geometry right down to the spiral threads on screws. If you have many screws in your design you might find that your CPU/memory gets bogged down, and your graphics processor works orders of magnitude more. While such detailed geometry is aesthetically appealing, IMHO it's not worth the degradation in performance of your computer. So, as I said before, cut it, dear Henry, cut it ...

  2. #12
    SOLIDWORKS Support Volunteer Tom Gagnon's Avatar
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    Not everything McMaster sells has models to download, but for fasteners it covers all that I've experienced. Jeffrey is correct that you have to locate the part and then click on the CAD Drawing link with a crosshair center mark icon. That is, there is no site menu item for download area: it's ordered by catalog, then downloads are either available for that part # or not.

    For threaded fasteners, I really prefer to download the Part so that I can suppress the thread cut feature. IIRC, it's usually a "Swept Cut" feature. It's nice that I haven't encountered any parts from there where subsequent features (in parent/children relation) rely on the thread being there. Otherwise, suppressing a parent will necessarily suppress its children. The part I find useful in assemblies at the scale I draw is a bolt with no thread shown as a cylinder with a hex head, a NPT (threaded pipe) socket expressed as a simple tapered smooth surface, etc. If drawing details with fasteners, you may want to unsuppress the features, which is doable with a part configuration in the part so you have a default and simple configs, or default and complex configs depending on what you'd normally use.

    Either way, decide and establish a pattern that will be followed in your use for all fasteners as Anna pointed out very importantly: file naming, Description syntax, units, configuration names, names of references such as "Axis" vs "Axis1" or "Long Axis", even orientation on the origin & primary reference planes should all be consistent in your pattern. These things are important to make your task easier when using Replace Components (with mates) command in an assembly, sorting parts in a Bill of Materials, and much more. This is a difficult lesson to care about when starting out learning other basics, but once you learn more you may decide to rework all the bits you've gathered.

    As a sidenote, beware of downloaded parts that are located far from their Origin. To me it shows that someone exported it from an assembly or a multibody part. Before saving or using any such part, I place the bodies onto the origin with constraints so it is more useful to describe relations in its use. I've never found McMaster to provide such boneheaded design parts, but the wider industrial market may choose to do things differently. (Example that comes to mind: Stahlin.com FRP electrical control panel enclosures.) Most often, if an item is modeled "on its back," that may be how it was manufactured, but not how it will be mounted to a wall or stand. It shows the manufacturer's design intent, not yours.

    Another comprehensive online resource, if narrowly specific, is Swagelok compression tubing fittings. Their entire catalog is available in multiformat downloads, but again they like to place the origin on the end of a part, not say the central intersection of a Tee fitting.

  3. #13

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    Thanks for the info on McMaster parts. I had forgotten about the link, because I never had software that could use it before! Now, my next dumb question refers to a comment made above about moving parts to the origin. I have been trying to determine how to do that and am completely stumped! How do you do it? Thanks in advance!

  4. #14
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Like many actions in SW there are several ways to do this:

    1. Go to Evaluate > Measure, on the body choose a vertex or center point that you want to be the origin of your part, and note the coordinates shown. Then go to Insert > Features > Move/Copy. Choose the body you want to move, and then as the reference point choose the point that you mesured previously. In the Translation boxes insert the negative values of the previously noted coordinates.

    2. Go to Insert > Features > Move/Copy directly, choose the body you want to move, and then Add mates to the three main planes (or any other geometry) that are located at the target location.

    3. If you have the history/feature tree then simply edit the first feature(s)/sketches so that they're located at your desired target.

    There are probably more ways to skin this cat.

  5. #15
    SOLIDWORKS Support Volunteer Jeffrey Meyer's Avatar
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    Quote Originally Posted by Tom Gagnon View Post
    For threaded fasteners, I really prefer to download the Part so that I can suppress the thread cut feature. IIRC, it's usually a "Swept Cut" feature. It's nice that I haven't encountered any parts from there where subsequent features (in parent/children relation) rely on the thread being there. Otherwise, suppressing a parent will necessarily suppress its children. The part I find useful in assemblies at the scale I draw is a bolt with no thread shown as a cylinder with a hex head, a NPT (threaded pipe) socket expressed as a simple tapered smooth surface, etc. If drawing details with fasteners, you may want to unsuppress the features, which is doable with a part configuration in the part so you have a default and simple configs, or default and complex configs depending on what you'd normally use.
    Here, here.
    I did a small experiment in this regard: I took a beautiful McMaster screw and exported an STL representation (STL is the file type used by most 3D printers - breaks the geometry down into thousands of triangular facets). The number of facets came out at 54,876. I then removed the detailed thread as suggested by Tom, and the exported STL representation produced 1,764 facets. This is a factor of more than 30. That means 30 times more computation of the geometry, 30 times more graphics computation, and a great deal more storage/memory.
    Thanks Tom.

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