Recreating odd shaped objects in CAD
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    Default Recreating odd shaped objects in CAD

    I was wondering how to recreate an odd shape in to a CAD file accurately. Are there any proper ways to do so? Here's an example img-3964.jpgimg-3962.jpg

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    I would start with a more regular shape and then cut away or use a revolve.

    Hard to get more detailed without the computer right in front of me.

    Sent from my SM-N950U using Tapatalk

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    How accurate do you need to be? ±0.001"? ±0.1"?
    The most you can generalize about is the problem of measuring to a certain tolerance, the actual how of making geometry in CAD is extremely object, CAD program and workflow-specific.

    For small-ish stuff (like under 1' in every dimension) that just needs to be "visually right", I'll often figure out a way to section (not literally cut, just measure/mark out) the object into multiple "slices" measurable with a caliper or other hand tool, then draw the measured sections and link those together with whatever geometry makes sense to use in Solidworks. The exact method depends on the size, shape and symmetry of the object. I do a lot of automotive trim type pieces this way. Someone who needs to hold tighter tolerances likely has a different method. Having a good rapid prototyping method helps a lot here, at least until you get really good (which I'm not).

    I've also used a Leica Disto to make point clouds of things that can then be used as references to drive models. Usually copious photographs and note-taking is required to make sure the point cloud data is properly interpreted. This is for furniture/architectural scaled stuff.

    I often have non-manufacturing people bring me a part to be reproduced and ask about "3D scanning" it. From my limited experience, unless you have really good scanning equipment and a super complex, detailed object (like a hand carved intricate scupltural surface), it is better and faster to just model it from scratch. A scan will need to be cleaned up and will not produce true straight lines/prismatic surfaces (most efficient for CNC programming) automatically. Take this with a grain of salt as I'm not up to date on the latest/best scanning tech, which I'm sure some others on here know better.

    Also, there is a CAD forum here, looking through some old discussions here might be helpful. https://www.practicalmachinist.com/vb/cad-cam/

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    For my task it only has to be around .1"+- so I think I'll try doing the multiple slices method that you've mentioned, thanks a lot for the input.

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    Most CAD packages have a couple handy features.

    One is the ability to "push" or "pull" surfaces. That can let you eyeball the thing into a good reproduction of a shape by "pounding the surfaces" into proper shape..

    The other, and more useful one is a variation of the slices, where you use guide curves to make an extrusion conform to a set of lines through the sections. Or, you may let the software create a shape with a surface that goes through each of the sections,

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    Quote Originally Posted by carbonbl View Post
    I often have non-manufacturing people bring me a part to be reproduced and ask about "3D scanning" it. From my limited experience, unless you have really good scanning equipment and a super complex, detailed object (like a hand carved intricate scupltural surface), it is better and faster to just model it from scratch. A scan will need to be cleaned up and will not produce true straight lines/prismatic surfaces (most efficient for CNC programming) automatically. Take this with a grain of salt as I'm not up to date on the latest/best scanning tech, which I'm sure some others on here know better.
    Photogrammetry (sp?) is a generic term for generating a model from a series of pictures - which is basically what some 3d scanning consists of, as best I understand it. I keep meaning to check it out - supposed to be FOSS programs to do this ... but whether the results are even vaguely usable is, as carbonbl points out, is another question.

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    I have been doing this for years. The cheapest way is to get yourself a Microscribe digitizing arm and a copy of Rhinoceros software. The software costs about $1,000, and allows you input points and splines with the Microscribe digitizing arm. The points are used to align your workpiece with the Microscribe arm. The splines are used to create the 3-d object, so that be used in a 3-d cad cam system like Mastercam. The accuracy of this drawing is within .009 of the actual part that you are trying to draw. You could also buy a Faro arm that would have a closer resolution compared to the Microscibe. My Microscribe arm cost me about $5,000, the Faro arm is about $12,000.

    Be aware that learning 3-d geometry will not be a simple process which you may or may not have the inclination or patience to master.

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    I didn't know about the push and pull abilities thanks.

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    Quote Originally Posted by food. View Post
    I didn't know about the push and pull abilities thanks.
    Not all CAD has that, and it does not work on all surfaces.... You will have to look and see if it is a feature for yours, and what it works on. I use Alibre, which has that.

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    You don't mention what CAD platform you have access to, but if you have Solidworks, the following works quite well. Lay the part on a copier or scanner that can output a jpeg file and take at least two scans with the part positioned 90 degrees from the 1st scan for the 2nd "picture". In SW, import the two scans into separate sketch pictures. Now you can sketch around the outline of the sketch picture to develop the shape in two perpendicular planes. If you go into Tools/Options and turn on Autotrace, this can make creating your sketch much easier- (there are multiple YouTube videos on this). Once you have your sketches made you can develop a lofted surface between the sketches. If you need better precision take some measurements of the part at different locations and tweak your sketch shapes to those control points. Have fun too!!

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    I have Inventor and Solidworks but that sounds really good I'll give it a try thanks so much.

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    That looks like a fairly simple sheet metal fabrication, but with a little stretching maybe. Is it possible to just template it with a few pieces of paper (wrap the paper over the item), scan the paper shapes, then pull the edges together in CAD?

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    If your CAD software has "loft" surface generation capability, there is a low-tech hybrid manual/CAD technique that will work well for parts like the one you pictured. That part has a generally fan-like shape, which will be natural to exploit in CAD. Take a marker and draw a some number (five?) of lines across the part, parallel to the "rim" of the fan. For simplicity, make these lines planar, so they only curve up and down.

    Now, using your favorite technique of CMM, surface plate work with a height gage, or cutting cardboard templates to fit, find out what those curves look like and bring them into your CAD SW. You probably don't need more than 6 to 8 points on each curve, but give each curve the same number of points. If you cut cardboard templates, spend a little time making sure the CAD curves look nicely like the whole curves you captured. Arrange them in 3D space as they are in the real world, and tell the SW to loft a surface through the curves. Adjust the rim to match the actual object, and then make your best effort to blend the corner/tip/base of fan. (That will probably be the task that requires the greatest skill with the CAD tool.)

    This technique works well for many classes of shapes, but it's not going to very helpful with highly "organic" shapes or reproducing Art Nouveau vinework, etc.


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