Solidworks to Mach3 Cutting Path

Discussion in 'Workshop Tips and Secrets / Tools' started by berridos, Nov 25, 2013.

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  1. Nov 25, 2013 #1

    berridos

    berridos

    berridos

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    Hi Guys

    The time approaches to cut my fuselage into styrofoam slices. Exactly 130 x2 2 inch slices.
    As I set up the first crosssection of the 130 crosssections it seems that the line segments are disjunct. I cannot add any relation to match the end of two line segments. Any idea on how to efficiently proceed? Besides that i want to use these drafts as cutting path and therefor pass them somehow over to Mach3 Any ideas? planos.jpg vision amplia.jpg primer corte.jpg
     
  2. Nov 25, 2013 #2

    DangerZone

    DangerZone

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    In metal CNC working a CAM program like MasterCAM or similar assists efficiently between a CAD program and Mach3. If a CAM program is not available or affordable, larger foam core jigs and templates can easily be cut with a foam cutter, specially where CNC is not practical.
     
  3. Nov 25, 2013 #3

    Jay Kempf

    Jay Kempf

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    You need something to turn your DXF or STL into something Mach3 can work from. Mach3 really only does XYZ coordinates.

    Your problems with your profiles are from the way you modeled the fuselage. You can see how the curvature is disjoint. In order to get a proper loft that obeys some mathematical rules you have to construct it that way from the start. If you don't have smooth curves as guide curves and profiles you will get all kinds of in and out bumps and transitions. I like to build my lofts out of relatively primative objects and then combine them and shell them at the end. The least amount of guide curves creates the most faithful geometry. You also have to learn to use pierce points instead of coincident points so that when you edit you don't have the model blow up. Most people learning to loft tie things down too many ways on the same curve. My favorite way to create fuselage is with a few key profiles and unless there is some reason not to just 4 points of the compass guide curves as longerons. That's assuming mostly oval and round profiles. I use splines for guide curves and I mirror them to make a full shape. I don't use the mirror function to make two fuselage halves either. I can always cut the final shape in half for CFD if I need a half model.
     
  4. Nov 26, 2013 #4

    berridos

    berridos

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    I would have loved to simplify the lofting but due to the design constraint the lofting went mad. Therefor i used an oval primary shape and cut it where all the wing fuse intersection fuzz started. One of the constraints was to broaden the fuse up to the trailing edge and have flat walls where the flap deploys. Than came the leading edge fillets on top..... i would say it is impossible to significantly simplyfy the lofting. Stangely efven the initial lofting with 4 bulkheads came out strangely imprecise and didnt match the upper and lower spline outlines.
    I will save the drafts as dxf and the look for some software to edit them. Accuracy of the process is secondary as at the end everything will be sanded by hand and corrected if necesary. I have posted the same question in cnc forums. Lets see what advice i ll get.
     
  5. Nov 26, 2013 #5

    Jay Kempf

    Jay Kempf

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    Solidworks for things like you are doing take some planning. If you randombly approach the way you model it you will get random results in terms of smoothness of surfaces and especially where you have critical transitions. You have to think about what you are doing in terms of regions on the surface of the loft and then reconcile each one of those pieces of geometry. Leave the fillets off to start if you can't get them controlled. You can always cut your plug up and add them later. There is always a way to simplify lofting. I am always amazed at how people approach the aerodynamic skin as something other than a math problem. Simple shapes work the best most of the time.
     
  6. Nov 26, 2013 #6

    harrisonaero

    harrisonaero

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    I would start by saving the entire solid as a parasolid to make it dumb. It's far far easier to work with this way since it doesn't have to compute parametric features.

    Put a hole through the center of your solid lengthwise so you can use that for your fixture (slide the sections down the shish kabob) and laminate.

    Then take your parasolid and start slicing and creating section views (use array function to sketch your section lines 2" apart). Save as DXF, nest, and then cut.

    Once you have all your sections on your fixture spray paint the whole surface with a foam safe paint. This lets you see the original surface so you don't sand below it.

    Good luck and share pictures :)
     
  7. Nov 26, 2013 #7

    JamesG

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    Have you looked posted this over on the Artsoft: Mach3 support forum yet? I think that there are a couple of topics about cross sectional models there.

    Are you trying to produce 3D models of each segment along with the contour between them to generate the tool paths to get the CNC cutter to reproduce them? Or do you just want the fore and aft loft lines? I think that the rudimentary "Lazy CAM" G-code generator that comes with Mach3 can handle something as simple as cutting cross sections. But I think you would have to create a separate .dfx file and process each of your 130 sections...

    Go bug Art.
     
  8. Nov 26, 2013 #8

    Jay Kempf

    Jay Kempf

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    Yup, individual dxfs is the easiest way. Import and convert to 2D paths. It would be more fun to do the 3D slices. I am currently building a largeish CNC rig that can do close to 60 x 60 x 12 to make 12" slices of things or large wing slices for tooling (neg) or cores.
     
  9. Nov 26, 2013 #9

    berridos

    berridos

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    thanks all for the inputs. I allready managed to get dxfs but i have to correct one for one for the discontinuities....(looks like it will take 100 hours copy pasting-kind of job i am talented in) Whats a parasolid? In my infinite ignorance I am currently working with surfaces. Shall I fill the whole ship and make it solid? How...?
     
  10. Nov 26, 2013 #10

    Jay Kempf

    Jay Kempf

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    Parasolids is just the Unigraphics version of DXF. DXF is an AutoCAD format. Same same. Most CNC software can import either. When JamesG said parasolids what he meant was just bring a solid lump with no history tree into the CNC prep portion of the software to get tool paths. At least I think that is what I was interpreting. You could write a macro to extract all the profiles. In other words automate the make plane at some offset from the last one and then do the intersection curve with the plane and then name them and put on a drawing and save as DXF. I normally put them all on the same drawing and then convert the whole drawing to DXF or STEP to hand off the the CNC guys. Most CNC software allows you to grab individual profiles off of one big DXF.
     
  11. Nov 26, 2013 #11

    JamesG

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    That was "harrison" with the Parasolids.

    @ Berridos:

    I'm going off old brain cells and may be mixing up my CAD programs, but I think in SW there is a "Make solid" or "heal" an object. Essentially what you have now in your drawing is the "skin", a bunch of vertexes that the program treats as such. So when you slice it into sections, they will be more like ribbons with a funny shape than layers of foam. This will make converting them into useful models to tell a CAM program how to cut foam harder. Also if you have any inconsistancies in the map of that skin, like triangles that don't line up. These can screw up creating solid models and confuse CAM programs.

    By converting to a solid, this is closer to what you are trying to actually model, a plug of foam that you want to slice up. When you cut them into sections, the program will automatically create fronts and backs and "close" the shape, so that when a CAM program starts thinking about how to generate G-code, it has an actual shape geometry to work with.

    Lots of more accurate programmatic maths behind the scenes to my above description. Like Jay said, in CAD how you draw something affects your results or even if you run into a "deadend".
     
  12. Nov 26, 2013 #12

    Hot Wings

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    There are lot of good Solidworks tutorials on Youtube. Learning from them has to be faster than 100 hours copy/paste?
    solidworks surfaces to solids - YouTube
     
  13. Nov 26, 2013 #13

    Jay Kempf

    Jay Kempf

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    I think he is showing that he already has a solid that has a square notch in the middle for the strong back he will put all the slices on. He is taking the larger of the outlines of each slice meaning he will sand down to the smaller profile effectively knocking the corner off. Normally when you export to another CAD format it turns your editable lump into a dumb lump without your original frames and control curves. I thought that was what you were telling him to do.

    You are right that there is a "thicken" command in SW to allow surfaces to be turned into solids as well as other ways to solidify a set of surfaces.
     
  14. Nov 26, 2013 #14

    1Bad88

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    I don't know the size of the CNC that you are using, but I would make my cross sections longitudinally if at all possible. Less modeling issues, less machining, less glue joints, etc.
     
  15. Dec 5, 2013 #15

    X'N

    X'N

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    I have a cnc router that I've been using for my bearhawk build.

    Check out Cut 3d from Vectric Products - Cut3D

    In solidworks save your model as a .stl Open that in cut 3d and you can section it how you want. While Cut 3d is on the lower end when it comes to 3d cam software it does work well but does not give you much control over cutting stratigies.

    Deskproto may be a better 3d cam software I hope to try it soon. DeskProto: 3D CNC machining for non-machinists. STL file milling for any CNC milling machine

    I tried mesh cam but didn't like that it didn't have a part preview built into the program, but it does give you more control than cut3d MeshCAM - CNC Software - CAD/CAM Software
     

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