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Thread: Kudos to the Solidworks Team

  1. #1
    rwanttaja's Avatar
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    Kudos to the Solidworks Team

    I've been ignoring this group all along, since I didn't have Solidworks or any real reason for a CAD tool.

    Then Santa gave me a 3-D printer for Christmas.

    Just wanted to say the download and installation were both flawless, and the built-in tutorials were a big help. Didn't take long to produce my first part generated from a Solidworks drawings.

    Well done, folks. And thanks to EAA for setting this up as a member benefit.

    Ron Wanttaja

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    You're welcome, Ron! The spectators on this forum love pics (e.g., SW drawings and printed parts). So if you find the time and care to share, please do! Thanks in advance!

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    rwanttaja's Avatar
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    Quote Originally Posted by Cory Puuri View Post
    You're welcome, Ron! The spectators on this forum love pics (e.g., SW drawings and printed parts). So if you find the time and care to share, please do! Thanks in advance!
    Be careful what you wish for. :-)

    My first non-practice part. 3/4 scale RAF Mark II reflecting gunsight, as used on the Spitfire, Hurricane. 3/4 scale to match the Fly Babies and Pietenpols of the world.

    A piece of thick plexiglass will be attached to the angle brackets to simulate the combining glass of the original sight; small pieces of angle will be bolted to the brackets to hold the glass just like in the original. I'll probably use plastic. Will see how the PLA material from the 3D printer handles a tap.

    The area is the middle has a stepped shelf for another piece of plexiglass to simulate the lens. I'm contemplating putting a black disk with a white aiming reticle under it; it may actually reflect a bit in the angled lens. In any case, it'll sit too low to actually be in the line of sight. It's designed to sit on a separate base to match the curve of the top of the Fly Baby's panel.

    The base was built per the tutorials included in the Solidworks package. The angle brackets were tougher; I could not come up with a way to do these in Solidworks (mind you, I'm a raw beginner...just downloaded the tool three days ago). Instead, I drew the shape in a standard 2D program (Canvas) and imported it into Solidworks as a DXF file. Did the normal extrusion just fine.

    Probably could have done this in a quarter of the time using a lathe and bandsaw, but was looking for a good excuse to play with Solidworks.

    Ron "What did you expect from me, spar fittings?" Wanttaja
    Last edited by rwanttaja; 01-04-2019 at 09:56 PM.

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    cwilliamrose's Avatar
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    Ron,

    Looks good. Extra credit of re-doing the angle brackets using the SWx tools only. Or post the model files and let us take a crack at it and we'll post our versions so you can see different approaches.......

  5. #5
    rwanttaja's Avatar
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    Quote Originally Posted by cwilliamrose View Post
    Looks good. Extra credit of re-doing the angle brackets using the SWx tools only.
    <Hangs head in shame> Yes, I cheated. The first problem was the tilted nature of the top part of the brackets. I'm presuming I need to create a new plane (or a pair of planes) for these. In addition, they're not simple geometrics; my first thought was to string together a group of lines but the DXF import was a heck of a lot easier.

    Finally, the *actual* brackets aren't simple extrusions...they taper at the bottom, where they attach to the base (kind of scalloped, in fact). So I need to create shape that's not symmetrical nor a standard extrusion.

    Two years ago, I worked with several bright-eyed engineers using ProEngineer on a daily basis, and would have been able to ask for help. Now that I'm retired, it'll cost me beer.

    As it sits, the model wasn't too compatible with the 3D printer (Dremel Ideabuilder); the slicer added a lot of supports to the angle brackets and they'd be a bit tedious to cut away. I've basically cut off the angle brackets just at the top of the base, and will print the brackets separately and see how well superglue works to put them in place. It'll make it easier to drill and tap for the glass-holding angles, too. Printer's singing happily away as I write.

    Quote Originally Posted by cwilliamrose View Post
    Or post the model files and let us take a crack at it and we'll post our versions so you can see different approaches.......
    What's the best way...a zip file with the .SLDASM and the .SLDPRT of the parts?

    Ron Wanttaja

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    cwilliamrose's Avatar
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    There's a function called "Pack and Go" which creates a full file set from an assembly.You can either put the file set on your local computer or have the function create a zip file containing all the necessary files. You'll want to check the file size to make sure it can be uploaded here. If the model is a single file you might be able the just upload it as an .SLDPRT file or have Pack and Go put the part file into a ZIP file for uploading.

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    rwanttaja's Avatar
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    Quote Originally Posted by cwilliamrose View Post
    There's a function called "Pack and Go" which creates a full file set from an assembly.You can either put the file set on your local computer or have the function create a zip file containing all the necessary files. You'll want to check the file size to make sure it can be uploaded here. If the model is a single file you might be able the just upload it as an .SLDPRT file or have Pack and Go put the part file into a ZIP file for uploading.
    The Zip file is 228K, forums have a 98K limit. I've put it up on a web page for downloading.

    http://www.bowersflybaby.com/sight.zip

    Be gentle with me. :-)

    Ron Wanttaja

  8. #8
    cwilliamrose's Avatar
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    That will work. I'll report back on Monday if I don't get to it tomorrow.

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    Just getting into your models Ron. Is the assembly a single part you will 3D print or is it meant to be separate parts in your application? I can do it either way but if you're planning to to print the part as one piece it should be modeled that way.

  10. #10
    cwilliamrose's Avatar
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    Here's a link to the one piece version I did.

    https://1drv.ms/u/s!AvtE9A43UNmAghi-bpbNbRJyN6gW

    And a screen shot;

    Name:  TEMP1.JPG
Views: 96
Size:  88.5 KB

    I have several comments on your models.

    First, you don't want to use multiple sketch entities to describe simple profiles. Your bracket has 25 entities (lines and splines but no arcs) where my cleaned up version has 14 lines and arcs, no splines. The problem with using so many entities in a profile is that each one creates a separate face which makes the model look cluttered and the file size will be larger to store all that extraneous data. Making a part or even a drawing of a part generated from a model like this becomes very difficult.

    What you want to do is the create the simplest possible profile sketch that has all the needed features and captures any design intent you feel is important. One question I had in cleaning up your profile was concerning the legs of the bracket -- the long one had pretty close to parallel sides but the short one had angled sides. I couldn't tell if that was an important part of the design or just the way the profile was originally drawn. I ended up making the longer one parallel and the shorter one with a 6 taper. The other thing you want to do is make the sketch easy to edit. Mine isn't too good because I was not sure what was important but it's much easier to deal with than your sketch would be because it's simpler and has dimensions and constraints fully describing each entity of the sketch. My sketch is fully defined (all entities are black) while yours is completely devoid of definition (all entities are blue). I can easily disturb your profile and cause it to change -- I can even do that unintentionally. Once that happens I can't put it back the way it was.

    If/when you want to use configurations you need to have dimensions driving the geometry so you can make new versions of your features by simply changing the dimensions.

    My model takes an average of what your model seemed to be doing. If it needs to change in any way it's easy to do so. Also, my part model is symmetrical where your assembly was not because there was nothing holding the various parts in place relative to each other. Again, it would be easy to disturb the assembly by mistake and not be able to get it back where it was originally. When you create an assembly each part needs to be mated to the other parts such that the assembly behaves like the real parts will when they are assembled.
    Last edited by cwilliamrose; 01-07-2019 at 09:39 AM.

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