Welcome to Our Community

Some features disabled for guests. Register Today.

how to cut the sides ?

Discussion in 'CAM' started by abdusalam, Jun 3, 2017.

  1. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    hi team :
    HOW I CAN DO IT BY sketchucam ?
    i am sorry because my English language weak:( so i hope someone understand my issue !
    i work on sketchucam , i have piece of aluminum ( for ex: 10cm*10cm*2cm high).
    i want the cnc to eat each side 2mm (to be squared ) all sides .
    the problem it is that the sketchucam work only on z axis to cut , i mean it cut from up to down only.
    but i want the cut from side to side like as the pictures show !
    ( i want the cut from side to side ,not from plunge .
    i have end mill 4 flute so i want to use it for cut the sides
    may be this video explain my needed :


    or this :

    HOW I CAN DO IT BY sketchucam ?
     

    Attached Files:

    • 11.PNG
      11.PNG
      File size:
      34.3 KB
      Views:
      4
    • 222.PNG
      222.PNG
      File size:
      55.5 KB
      Views:
      5
    #1 abdusalam, Jun 3, 2017
    Last edited: Jun 3, 2017
  2. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    how?
     
  3. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    i try with inside cut and with outside cut and with boundary cut but not work
    i want multi side cut (side by side ) instead plunge multi cut!
     
  4. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    SketchUcam has no knowledge of the outside of the final piece since it is designed around cutting shapes from a large sheet of flat stock. (see 'Phlatprinter' on youtube)

    so, my method for squaring your bit of stock.....
    1. Draw the rectangle of the final size you want.
    2. draw a larger rectangle around it (leaving some extra space beyond your stock, depending on your bit size)
    3. 'pocket FLOOD' the space between.
    4. delete the outer rectangle cut.
    5. group the zigzags together so they cut first.

    I found it better to rotate the rectangles 45 degrees before pocketing. then rotate them back.
    This gives a safer zigzag cut that will not cut a full depth cut along an edge since it is all at an angle to hte edges.
    squarethestock.png

    Remember to turn on RAMPing and set the right angle when cutting aluminum.
     

    Attached Files:

    MaryD and Joe Santarsiero like this.
  5. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    thanks David
    is this cut from side to side or from up to down ? i mean : did you see the second video at 00:49 ?
    the end mill not plunge from up to down in the piece , it is cut from side to side .
    * you mention me about ramping in z ! the ramping i used when i plunge at the surface of the piece only (not at sides i think)
    could you please make video to explain how cut the sides of stock by sketchucam
     
  6. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    Did you download the file I posted and run the gcode? Use a 6mm bit and cut a piece of insulation foam, then you will see what it does and gain understanding.

    Sketchucam does not do cuts like those shown in the video. Those are called HSM paths. If you really need those, and have a 10horse power mill that can do it, then maybe you need Fusion360? In Sketchucam You could draw lines by hand and then set them as centerline cuts, then do a finishing pass with an outside cut. This is tricky to get right.

    Meanwhile, please watch these videos and read the manual so you can better understand this tool...
    Phlatboyz SketchUcam Help

     
    abdusalam likes this.
  7. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    Did you download the file I posted and run the gcode?
    *not yet ...but i will do it soon.

    Sketchucam does not do cuts like those shown in the video. Those are called HSM paths. If you really need those, and have a 10horse power mill that can do it, then maybe you need Fusion360? In Sketchucam You could draw lines by hand and then set them as centerline cuts, then do a finishing pass with an outside cut. This is tricky to get right.
    yes ...that's what i want to know ...i have to do some modification to do some cuts because the sketchucam not support it.) am i right?

    i red all help and watched all video on you tube ....and test them all so i start to get some experience too ...but i ask to make sure of some wondering.
    *********************************************************************************************************************************************************************
    now about spindle power :
    my spindle has 1.5kw ...i know it is not good for some cuts ..but all i want it is to cut just 1mm from side ...i think i do nor need 10hp to cut just 1mm from side
    why i need to cut from side instead plunge with end mill ? ..because i have None center cutting endmills. so i can not cut from up.

    please correct my answer if i am wrong !!
    thanks David
     
  8. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    other question : how control the cuts direction or cut start point ? please see my small example :
    see the picture :
    i draw rectangle and made 4 offset with 2 distance between them ...so
    the outer rectangle No. (1) its is the true size of my piece
    the fourth rectangle (4) it is the final size i want ( my objective )
    the second and the third it is just steps to reach my final shape
    NOW ... i made outside cut tool for all rectangles .
    the problem it is that the toolpath start from inside rectangle , not from out side
    how i can change the start cut to be from outside to inside ?
     

    Attached Files:

    • cut.PNG
      cut.PNG
      File size:
      418.5 KB
      Views:
      2
  9. Giarc

    Giarc Master
    Builder

    Joined:
    Jan 24, 2015
    Messages:
    518
    Likes Received:
    249
    You could just make four separate g code files and run the outside one first, then work your way in to the final size by running each file. Or make them separately then join them to run as one file.
     
    abdusalam likes this.
  10. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    yes you right ..that will be the last way ...i am looking for more easy way
     
  11. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    how i can change the direction of cut ? to do (climbing cut) ......i think the sketchucam are weak to make some professional cuts. ( may i am in wrong ) but i still learning.
    please guys be patient with me
     
  12. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    RAMPING solves this! SketchUcam: HOWTO use Ramping

    There are situations where it cannot ramp and will convert to a plunge (when the line segment is too short). There is always a warning comment in the Gcode when this happens, so you just need to read the Gcode and check for warnings.
    Code:
    G00 Z5.000
     X12.278 Y10.566
    G01 Z-6.300 F1000
    (ramplimit end, translated to plunge)
     X12.060 Y11.045 F2000
     X11.454 Y12.123
    
    The line just before that warning shows that it is plunging down to -6.3mm, you have to prevent that.

    The optimizer does search for a long enough segment for the ramp and will only plunge if one cannot be found. If your shape does not have any long segments then you will have to pre-drill a hole for the tool to enter (using a real drill bit of course).

    What is long enough to ramp? A segment must be longer than the bit radius. This allows for tools where the end cutting edge is larger than half the radius to be ramped. If the cutting edge is smaller than half the radius, then it will get jammed on such a short segment.

    To force a cut to start at a desired place you can place a plunge hole near the start point you want, then group the hole and the cutline.
    Why does this work?
    Because groups cut in group order.
    The plunge hole is a group.
    So when it is grouped together with another cutline, the hole will cut first, then the cutline.
    The optimizer starts the cut at the closest point to the last cut end point.
    But, you don't want a hole, so make it 1% deep. 1% of 10mm thick material is 0.1mm. If that makes too much of a mark, you can search and replace that depth in the Gcode to prevent any tool touch.
     
    abdusalam likes this.
  13. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    You said you read the help, and the answer to this is in the help.
    SketchUcam Toolbar
     
    abdusalam likes this.
  14. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    hard to help you more until you have studied that file and run that code.

    You can simulate the Gcode with this
    CAMotics
    so you can see where the tool is moving without running the actual machine, but I still prefer the 'cut some insulation foam' method (-:
     
    abdusalam likes this.
  15. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    To do the cut shown in the video, you probably need more power. This is because it is cutting about 30mm deep in one pass.
    Even though the side to side cut depth is very small, 30mm of tool engagement takes a lot of power (and a stiff, heavy machine).

    So, 1.5kw means you cannot do a cut exactly like the one in the video, but you will be able to do it in multipass layers.

    What machine do you have?
     
    abdusalam likes this.
  16. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    The answer is 'groups'....
    SketchUcam Toolbar
     
    abdusalam likes this.
  17. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    thanks David
    the conversation with you gave me more experience
    my machine (diy) i build it on my own :D see picture.
     

    Attached Files:

    • 63.PNG
      63.PNG
      File size:
      880.7 KB
      Views:
      7
    David the swarfer likes this.
  18. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    about the g-code ....i ran the g-code .....
    do you mean the endmill will cut the side by zigzag ?
    the end mill eats the side with same way you draw zig zag ...i think finally understood your way
    again :
    see the picture please :
    No 1 means the cut done
    No 0 means the cut not done
    the edge of the piece become some cut and other not cut because it follow the zigzag line as in picture
    so we need the boundary line to cut the rest of zigzag ...
    all the way ...thank you very much M.S:David
    you gave me many ideas to go ...so i will try your way and i will edit it to cut in good way ...
     

    Attached Files:

    • 012.PNG
      012.PNG
      File size:
      29.6 KB
      Views:
      1
  19. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    well, I don't know what you are doing. The cuts I drew will do:
    the zigzag to remove most of the material from the edge
    then a final cut to clean the surface

    upload_2017-6-7_8-48-32.png
    the zigzag is purple
    the final cut is blue (because I selected it to highlight it)
    That is a continuous straight line cut all the way around the part to clean the edge. (and it can be seen in your picture!)

    so there are 2 cuts. If you only got a zigzag, then you must have selected it before generating Gcode.
    You should get 2 cuts and a clean edge.
    Make sure you have nothing selected when you generate the Gcode.
     
  20. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    Here is what I see in simulation
    (watch the attached video)
     

    Attached Files:

  21. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    yes ...exactly ..that what i meant ( but i could not explain it with English exactly:cry:).....it is works good .
    cause of your help , i found other way ..it is very easy and new ( i think no one know it :p:cool: ) i will post the new way here ....just after make some test .
    thanks thanks thanks ...all my issue finished.
     
  22. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    David the swarfer :ROFL::ROFL::ROFL::ROFL:
    finally...i control on the path tool ...now the end mill can start from outside and goes to inside edges ( one by one) pleas run the g-code in attachment inCAMotics and see the toolpath .
    the inner shape it is the final shape and the outer it is the new piece that i want to machine it .
    so i can also make the end mill start from inner to outer .
    did I make discover or no thing is new ?
    if that is new for the builders , i will explain my way !
    and i hope put your comment about this
    note : this way without join multi code files...just one run
     

    Attached Files:

    #22 abdusalam, Jun 7, 2017
    Last edited: Jun 7, 2017
  23. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    775
    Likes Received:
    357
    Both your files have warnings in them and the Gcode is not really valid.
    Code:
    G90 G21 G49 G17 G61 F2540
    M3 S15000
    (RETRACT limiting Z to @max_z)    <---- this is a problem!
    G00 Z0.000
    (RETRACT limiting Z to @max_z)
     Z0.000
    G01 X105.054 Y312.356 F6500
     Z-3.000 F2540
     X415.054 F6500
     Y622.356
     X105.054
     Y312.356
    (RETRACT limiting Z to @max_z)
    G00 Z0.000
    G01 X106.054 Y313.356
     Z-3.000 F2540
    
    (RETRACT limiting Z to @max_z) is a warning that you have not correctly set your MAX_Z value or are using material thickness + safe height that is too high.
    However, I believe it is set to 0 which is WRONG, MAX_Z must be set to the distance your Z can travel otherwise it cannot lift to a safe height above the work (since the work surface is Z=0).
    MIN_Z must be negative Z travel to allow it to travel below the work surface.

    Urgently go and read this
    SketchUcam - Thing to do After Instal
    and fix your settings!

    Note that the Min_z and Max_z settings are not foolproof in preventing machine crashes.
    If you are machining thick parts you need to think about the clearance and Z travel limits.
     
  24. abdusalam

    abdusalam Well-Known
    Builder

    Joined:
    Jun 1, 2017
    Messages:
    18
    Likes Received:
    1
    ohh... i forget to tell you that i have 2 pc ....one in workshop that connect with cnc ....and other in my flat ( that i write from it to you now ) this pc ( sketchucam) not correctly setting and just for test some generate g-code ........
    i mean , do not care about these warning .
     

Share This Page