584,805 active members*
5,127 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 26
  1. #1
    Join Date
    Feb 2009
    Posts
    129

    First Try From Image

    So this is my first attempt to mill something from an image.
    It actually came out better than I thought it would. But I would
    like to be able to do it much better.
    The pattern is an inch by an inch and the cutter was a 1/16 inch ball.
    I wish I could remember what the step over was but I don't remember.

    So to make it better I am thinking that if I decrease the step over distance
    I should get the circles to appear more round and probably improve the
    shape of the text?

    Then I got to thinking that if I went to say a 1/32 ball I should be able to get the text to cut deeper and improve the look, but that means the step over will have to be like 4 times as short right?
    Attached Thumbnails Attached Thumbnails 3D1.jpg   3D2.jpg  

  2. #2
    Join Date
    Nov 2008
    Posts
    113
    Looks pretty good really,

    Try a 4-8% step over (translates to about 0.0025"-0.005" ridges) and try a square end end mill. You actually don't need a ball end unless you have features that require it.

    This to me looks like a height map generated by an image with a lot of contrast where the edges between the circles and the background a very crisp. This type of image doesn't really require a ball-end mill and will cut down on ridges on the back of the plate.

    Now if you decide to do something complicated like a portrait then the ball end mill would be necessary.

    What software are you using to generate the gcode?

  3. #3
    Join Date
    Feb 2009
    Posts
    129
    Interesting idea about the flat mill. I can see how that would be a good idea for this part.

    I actually want to do much more complex ones though. I just did a real simple shallow one cause I didn't have much time to wait around while it cut last night.

    I'll try it again tonight with something a little more complex and see how it goes with 4-8%.
    Thanks!

  4. #4
    Join Date
    May 2009
    Posts
    43
    That is really cool. I'm also interested in how you did that and with what software? Does the software do most of the work, or is there a bit of a learning curve to get 2D images to 3D shapes?

    I'm planning to cut a gargoyle shape from vectorart3D when I get my machine built, but I would like to learn how to do what you're doing and be able to create these shapes myself.

  5. #5
    Join Date
    Feb 2009
    Posts
    129
    It was pretty easy actually, I just made a gray scale jpeg and opened it in Meshcam.

    There are a lot of settings to play around with, and I am sure that I can get it to come out way better by messing around with the settings some more. Of course I expect it to take a lot longer to cut it out in order to have it come out nicer...

  6. #6
    Join Date
    Feb 2009
    Posts
    129
    I did it with photoshop and meshcam.
    It was pretty easy. Especially compared to writing all the gcode for it out by hand!
    It came out to about 48000 lines of code!

    I'm going to try another one tonight, i'll post the results.

  7. #7
    Join Date
    May 2009
    Posts
    43
    Very cool! I'll look forward to seeing your next part.

    When you are playing with step over distance and cutter sizes, do you have to scrap the part each time you try something different? Or, can you see that you want a little sharper detail and reprogram and run on the same part with smaller step over to smooth it out?

  8. #8
    Join Date
    Feb 2009
    Posts
    129
    you could do a test area on the part, somewhere that you were going to cut away anyway. You could put in a circle and see how it comes out before doing the whole pattern. Once you get a feel for what the settings should be you probably don't need
    to though. I was thinking that if the one I did last night didn't come out that I would just mill it flat and start again. But I will probably keep it so I can have a reminder of my progress. This milling stuff has no end to things to learn!

  9. #9
    Join Date
    Dec 2008
    Posts
    445
    You've obviously got the software you've got, so you can take this with a grain of salt. There are a couple of things that will influence the results you get. The square end (or a smaller ball mill to some degree) will give you steeper edges per a given cut depth. That will improve things a bit.
    The other thing that would help is a machining strategy that does a better job at following arcs and such instead of just generating a straight raster cut. Here is where you are limited by meshcam I'm guessing. Given that a smaller end mill and smaller stepovers will certainly help. I do some mold cutting, and I use a constant 3 dimensional stepover cut of .001 or .002 and get a great finish, it does take a little while though.
    I'm not sure exactly how meshcam maps pixels of an image to features size in the final part, but there may also be some stair stepping introduced as part of the attempt to map one to the other. Might be worth a look, although it's just a theory, as I said I don't know the software.

  10. #10
    Join Date
    May 2009
    Posts
    43
    This makes sense. You could cut the top and the floor with a square end mill. Then, go around the contours with the ball nose instead of sweeping straight lines back and forth. Is that even possible? I'm just now starting to realize how much I have to learn, haha.

  11. #11
    Join Date
    Nov 2008
    Posts
    522
    The smaller mill does not make smoother features.
    The smaller mill allows you to make smaller features than a mill which is wider than the feature.

    With fixed parallel stepovers (raster output), the smaller mill leaves a bigger cusp as it climbs vertically. This can be reduced by using smaller steps and extending the milling time. However, even if you reduced the stepover by half, the cusps on nonhorizontal surfaces will always be present just reduced. And they will always be smaller if you use a larger mill.

    In short choose the largest mill that can still render the features. In some cases it makes sense to do a tool change to render just the fine features with a smaller mill.

  12. #12
    Join Date
    Feb 2009
    Posts
    129
    I see what you are saying about using the biggest mill that will work.
    I am timid about doing a change on a program like this though. How would I ensure that the Z is the same between the tools? I would like to try it though, maybe I will give it a try tonight.

    I tried a much more complex image last night.
    The details were too small for my 1/16 mill so most of the detail didn't come out.
    I guess there was also a problem with the way I told meshcam about the size and or location of the material because even though the Z0 level on the mill was actually
    set below the top of the material it still didn't cut the highest details.

    I wanted the Z 0 that I set to be the actual top of the piece after it was done.

    Anyway, here is a picture of the result and also the image file that I put into meshcam.

    I think I might try doing the models in 3D instead of trying to do these gray scale images. I don't feel like I have as much control as I would like with the images.


    Mini Beast- Yeah there really is a lot to learn. There are a lot of places that problems can come from that lead to unexpected results. It is sort of overwhelming because you really need to learn how to machine things, how mach3 will handle the gcode, how to generate the gcode and how to make the drawing or model to give the cam software. I think that most people who get into this sport already know how to do one or two of these operations and that is a help. But getting all of these operations to merge smoothly into the joining ones is a juggling act for sure! Still it is AMAZING to watch the cutter shape the material. I literally sat and watched it last night for an hour and a half as it revealed the new shapes each pass. Memorized like a kid at a magic show!
    Attached Thumbnails Attached Thumbnails heart_sample_2.jpg   heart_sample_3.jpg   heart_sample_4.jpg  

  13. #13
    Join Date
    Nov 2008
    Posts
    522
    Quote Originally Posted by 5artist5 View Post
    I am timid about doing a change on a program like this though. How would I ensure that the Z is the same between the tools? I would like to try it though, maybe I will give it a try tonight.
    IF you've got collar-set bits with the same 1/8" shank, the tips should in theory be at the same point when you change. The collar surface which goes flush against the chuck is precision-placed a standard distance from the cutting tip.

    [QUOTE=5artist5;615009]I tried a much more complex image last night.
    The details were too small for my 1/16 mill so most of the detail didn't come out.
    I guess there was also a problem with the way I told meshcam about the size and or location of the material because even though the Z0 level on the mill was actually
    set below the top of the material it still didn't cut the highest details.

    Neat. How deep did you ask the software to go?

  14. #14
    Join Date
    Feb 2009
    Posts
    129
    Quote Originally Posted by MechanoMan View Post
    How deep did you ask the software to go?
    I think i told it to cut .125"


    Who sells collar set bits? That sounds perfect.


    I actually have some collars that I bought to try to set up the same sort of thing but I haven't tried it yet. I need to come up with a good way to set all the collars the same.

  15. #15
    Join Date
    Feb 2009
    Posts
    129
    Quote Originally Posted by escott76 View Post
    You've obviously got the software you've got, so you can take this with a grain of salt.
    I was thinking about what you said escott76. I am actually using the demo of meshcam right now. Is there some other software that works better for this kind of thing?

  16. #16
    Join Date
    Dec 2008
    Posts
    445
    Quote Originally Posted by 5artist5 View Post
    I was thinking about what you said escott76. I am actually using the demo of meshcam right now. Is there some other software that works better for this kind of thing?
    There are plenty of pieces of software that will work better for this. They are gonna cost a bit of money though, and require some more work to learn.
    The best results aren't going to come from using an image to generate toolpaths from, but rather solid models, or even geometrical representations of the part in 2D that define machining boundaries. You would then use CAM software to pick out the areas and pick machining types to go after them.
    If it were me I'd take the graphic, import it into Solidworks, draw geometry over it and create a solid. Then I'd import the solid into GibbsCAM and go from there. But not everyone has such tools available.
    It appears as if you are trying to do finer work, such as jewelry. Using an image to generate the tool paths may not be the best way to get the kind of look you are looking for. I have personally hand coded things of a similar nature to your first effort by fitting lines and arcs to the areas to be machined, and then using the machine I was working with's "pocket" function to clear the areas. Time consuming yes, but it got the job done.

  17. #17
    Join Date
    Feb 2009
    Posts
    129
    Oh, i didn't realize that I can bring images into solidworks. That seems like a geat way to go. I am fairly comfortable making mechanical type parts in solidworks. But I always do them from either an external drawing or even from a part itself.

    Thanks for the heads up!

  18. #18
    Join Date
    May 2009
    Posts
    43
    When you are in sketch mode in Solidworks, go to Tools --> Sketch Tools --> Sketch Picture...

    As far as I know the picture can't be used to create entities, and it won't be on the model you export as .igs or .stl or whatever. I've used this before by just "tracing" over it with normal sketch entities basically like putting a blank sheet of paper over a photo and tracing over the image.

    I've done this before to make simple 2D contour type features. However, I think Solidworks would be very limited in making 3D type of shapes off an image compared to the art design types of software. I'm pretty good with SolidWorks, but I've never tried to do something like that. That's why I'm buying this to make my machine's name/logo plate. I wanted something 3D

  19. #19
    Join Date
    Nov 2008
    Posts
    113
    If you don't want to spend any money, you can try inkscape (you'll need to hunt down the "better dxf export" plugin) to redraw the image as a vector. You can then probably use meshcam, or the free version of CamBam to create paths. Will take some scaling work to get everything to the right size from inkscape but it does work -- I've done it a few times.

    You can also look in to programs that'll convert raster to vector, I've never used one so I don't really have any idea how well it'd work or if the resulting vectors will confuse your cam program, but its an option, and I'm sure theres something opensource (aka it works but you have to try harder ) that'll do the trick.

  20. #20
    Join Date
    Nov 2008
    Posts
    522
    Mach3's LazyCam has a tool for maching images as a depth map too.

    AFAIK, it can't handle non-cylindrical "V" engravers. Those are nice in that they can do crazy fine features. Like I've got one with a 6 mil tip. It can do ~6mil details. You won't find that in an endmill because it will be structurally unsound, just break off. However, they must run very slowly. At 10,000 rpm, a 1/8" cylindrical endmill sweeps past the material at 3925 inches per min (pi*diameter*rpm). A 6 mil dia tip is only sweeping past at 188.4 ipm at the very tip at 10,000 rpm!

    In fact, there is a very significant difference in climb vs conventional milling at this speed due to the resulting surface speed alone. If you're running at 20 ipm, the conventional milling gets a surface speed of 208.4 ipm, climb milling gets a speed of 168.4ipm. 20ipm is not "normally" unreasonable in plastic, or in aluminum metal where you're not cutting very deeply with each pass, but this factor may make it unreasonable.

    This is kinda why I wanna try one of these 30,000 rpm commercial spindles! Tiny tools going very very fast to achieve much better surface speeds.

    Anyhow, here's another thing: LazyCam, and some other tools, DON'T seem to be able to support V-engravers. You have to have a check to see that the side of the engraver won't remove what is supposed to be part of the remaining work, rather than always put the tip at the desired depth. MeshCam DOES do this if you define the tool properly. LazyCam and others cannot.

Page 1 of 2 12

Similar Threads

  1. Image Creation
    By rweatherly in forum Coding
    Replies: 3
    Last Post: 03-14-2014, 07:28 AM
  2. mirror image
    By cp465vw in forum Machines running Mach Software
    Replies: 8
    Last Post: 04-14-2009, 04:39 AM
  3. mirror image
    By blouie in forum Esprit
    Replies: 5
    Last Post: 12-24-2007, 08:24 AM
  4. image files to dxf
    By Goran P. in forum Mastercam
    Replies: 2
    Last Post: 07-10-2006, 03:54 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •