Offset cutting in Mach 4 how to di this


Results 1 to 17 of 17

Thread: Offset cutting in Mach 4 how to di this

  1. #1
    Member
    Join Date
    Sep 2010
    Location
    Aruba
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Offset cutting in Mach 4 how to di this

    Good day.
    if I have a shape that needs to be cut out for example a square with width is 30mm.
    After cutting and testing the part wont fit and I need to make it 31mm width...what would be the best way to tackle this? in Mach 4 without having to redraw again and import.

    Thank you!

    Similar Threads:


  2. #2
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by Matadem View Post
    Good day.
    if I have a shape that needs to be cut out for example a square with width is 30mm.
    After cutting and testing the part wont fit and I need to make it 31mm width...what would be the best way to tackle this? in Mach 4 without having to redraw again and import.

    Thank you!
    You could change the Tool diameter in the Cam program and repost it, so if you tool is 6mm change it to 6.5mm in the software repost the program and recut the part, you use the same tool in the machine, but the program thinks it is bigger and will cut .5mm larger each side, so this is simple to do, this is for outside a part if it is inside the and you want the pocket bigger post the cutter as smaller to make the pocket larger

    You could also use cutter comp G40 G41 G42 in your program and then change this Tool offset in the control. either way you still have to redo your program to use cutter comp

    Mactec54


  3. #3
    Member
    Join Date
    Sep 2010
    Location
    Aruba
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Thank you!

    Going to give it a try.



  4. #4
    Member
    Join Date
    Sep 2010
    Location
    Aruba
    Posts
    8
    Downloads
    0
    Uploads
    0

    Question Re: Offset cutting in Mach 4 how to di this

    Man I really need some help here...
    I tried change the tool diameter in the tool table then add g42 which I have read somewhere if you do not put anything behind it will use the info in the tool table.
    When I try to run it in Mach 4 the spindle start and just stays there it just stays stuck in one line.
    I tried the g42 D1 that supposed to read the tool table again it stays stuck. I added an attachment with the code that I use to cut a sample square if some one could point me in the right direction.

    Today I had to cut some squares and they came out about 0.8mm too small so after the cut I zero I moved the machine in the x 0.0314" zero it and recut so the items could fit. but in the x axis some trimming was needed.

    I have measured the bit white side upcut and it's dead on at 0.250". I am trying to figure this out since I am sure I will be stuck in the same situation in the future and also before I add the plasma addition which arrived today.

    Thank you!

    Attached Files Attached Files


  5. #5
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by Matadem View Post
    Man I really need some help here...
    I tried change the tool diameter in the tool table then add g42 which I have read somewhere if you do not put anything behind it will use the info in the tool table.
    When I try to run it in Mach 4 the spindle start and just stays there it just stays stuck in one line.
    I tried the g42 D1 that supposed to read the tool table again it stays stuck. I added an attachment with the code that I use to cut a sample square if some one could point me in the right direction.

    Today I had to cut some squares and they came out about 0.8mm too small so after the cut I zero I moved the machine in the x 0.0314" zero it and recut so the items could fit. but in the x axis some trimming was needed.

    I have measured the bit white side upcut and it's dead on at 0.250". I am trying to figure this out since I am sure I will be stuck in the same situation in the future and also before I add the plasma addition which arrived today.

    Thank you!
    Can you post a Photo of what you are trying to do the program does not look correct or the dimensions of the finished pocket

    Are you using absolute G90 for your programing or is it doing incremental G91 you can remove the G91.1 and see if it makes a difference

    Mactec54


  6. #6
    Member
    Join Date
    Sep 2010
    Location
    Aruba
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Good day the attached file had no modifications it comes straight out of vectric.
    attached is a pic of a the test piece.

    Maybe tool wear compensation will work ..but I do not know how to use it :/.

    Thank you!

    Attached Thumbnails Attached Thumbnails Offset cutting in Mach 4 how to di this-square-test-jpg  


  7. #7
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by Matadem View Post
    Good day the attached file had no modifications it comes straight out of vectric.
    attached is a pic of a the test piece.

    Maybe tool wear compensation will work ..but I do not know how to use it :/.

    Thank you!
    Cutter comp can be used but it has to be applied correctly in the program or it will either do nothing or make a mess

    So, is the pocket size 1.969 x1.969

    Try this program same setup as what you did

    Attached Files Attached Files
    Mactec54


  8. #8
    Member
    Join Date
    Jan 2018
    Location
    United Kingdom
    Posts
    1516
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Matadem View Post
    Good day.
    if I have a shape that needs to be cut out for example a square with width is 30mm.
    After cutting and testing the part wont fit and I need to make it 31mm width...what would be the best way to tackle this? in Mach 4 without having to redraw again and import.

    Thank you!
    Should've just set cam as 'stock to leave' 0.5mm and reposted it.
    It would have left 0.5mm on the part all around it making it 31mm.



  9. #9
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by dazp1976 View Post
    Should've just set cam as 'stock to leave' 0.5mm and reposted it.
    It would have left 0.5mm on the part all around it making it 31mm.
    To leave .5 would make the pocket smaller, you would have to post it as a -.5 to make it larger, he is working in inches by the program so would be a -0.019685

    It's just the same if you change the tool size to get the offset needed

    Mactec54


  10. #10
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    1567
    Downloads
    5
    Uploads
    2

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by Matadem View Post
    Good day the attached file had no modifications it comes straight out of vectric

    Thank you!
    ...there proabilly is a Setting in Vectric Cam output for Cutter Comp and must set for each Tool for left or right or none. None being default most likely.


    N10G00 G94 G20 G17 G90 G40 G49 G80
    N20G91.1
    N30T1M6
    N40M07
    N50G00 G43Z0.8000H1
    N60S20000M03
    (Toolpath: Pocket square test Tool: End Mill {1/4"} Whiteside RU2075)
    N70X0.0000Y0.0000F160.0


    N80G00X-0.1354Y-0.1354Z0.2000 ---change to N80G01G41D1X-0.1354Y-0.1354Z0.2000

    (LINE 80 Change G00 TO G01 and add G41D1 for climb cut )


    N90G1Z0.0000F30.0
    N100G1Z-0.1969
    N110G1X-0.0624Y-0.0624F160.0
    N120G1X0.0624
    N130G1X0.1354Y-0.1354
    N140G1X0.0624Y-0.0624
    N150G1Y0.0624

    Attached Files Attached Files


  11. #11
    Member
    Join Date
    Jan 2018
    Location
    United Kingdom
    Posts
    1516
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by mactec54 View Post
    To leave .5 would make the pocket smaller, you would have to post it as a -.5 to make it larger, he is working in inches by the program so would be a -0.019685

    It's just the same if you change the tool size to get the offset needed
    Depends if tool offset is playing well.

    You know what I meant. So, clarity..
    If it's an interal pocket needing hole to be 1mm bigger you'd leave -0.5mm.
    If it's around the outer edge needing to be 1mm bigger you'd leave +0.5mm.



  12. #12
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by dazp1976 View Post
    Depends if tool offset is playing well.

    You know what I meant. So, clarity..
    If it's an interal pocket needing hole to be 1mm bigger you'd leave -0.5mm.
    If it's around the outer edge needing to be 1mm bigger you'd leave +0.5mm.
    Does not depend on anything it's a calculation and is always correct, he is making a pocket to make it bigger you would use a negative number to make it smaller you would use a positive number

    Mactec54


  13. #13
    Member
    Join Date
    Jan 2018
    Location
    United Kingdom
    Posts
    1516
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by mactec54 View Post
    Does not depend on anything it's a calculation and is always correct, he is making a pocket to make it bigger you would use a negative number to make it smaller you would use a positive number
    Actually. Have a question for you while here.
    What's a reliable way to measure cutter diameter out of the box?. (apart from wasting material using the square cut method). Saves doing most of the offset adjustment discussed here.
    4 flute aren't so bad but I find 3 flute are a bit tricky and most end mills I use are 3 flute.
    Ta.
    Daz.



  14. #14
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by dazp1976 View Post
    Actually. Have a question for you while here.
    What's a reliable way to measure cutter diameter out of the box?. (apart from wasting material using the square cut method). Saves doing most of the offset adjustment discussed here.
    4 flute aren't so bad but I find 3 flute are a bit tricky and most end mills I use are 3 flute.
    Ta.
    Daz.
    There are a number of ways to do this, from lasers to anvil micrometer, you can use a height gauge with a V-Block and a drop indicator or a Gauge Stand like the snip with a V-Block

    Attached Thumbnails Attached Thumbnails Offset cutting in Mach 4 how to di this-gauge-stand-indicator-png  
    Mactec54


  15. #15
    Member
    Join Date
    Sep 2010
    Location
    Aruba
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by machinehop5 View Post
    ...there proabilly is a Setting in Vectric Cam output for Cutter Comp and must set for each Tool for left or right or none. None being default most likely.


    N10G00 G94 G20 G17 G90 G40 G49 G80
    N20G91.1
    N30T1M6
    N40M07
    N50G00 G43Z0.8000H1
    N60S20000M03
    (Toolpath: Pocket square test Tool: End Mill {1/4"} Whiteside RU2075)
    N70X0.0000Y0.0000F160.0


    N80G00X-0.1354Y-0.1354Z0.2000 ---change to N80G01G41D1X-0.1354Y-0.1354Z0.2000

    (LINE 80 Change G00 TO G01 and add G41D1 for climb cut )


    N90G1Z0.0000F30.0
    N100G1Z-0.1969
    N110G1X-0.0624Y-0.0624F160.0
    N120G1X0.0624
    N130G1X0.1354Y-0.1354
    N140G1X0.0624Y-0.0624
    N150G1Y0.0624

    I am going to do some tests tomorrow.
    this is not just about the square...but any other design to be cut and need some modifications.

    The main reason for this is my mach 4 pc is in the shop and my vectric pc is inside the house.
    I could redraw it in vectric with the compensation needed after measuring but going back and forward is not efficient.

    If I am already in the shop and in front of the mach 4 computer and making adjustments on the fly would be a great time saver.

    Attached Thumbnails Attached Thumbnails Offset cutting in Mach 4 how to di this-vpass-jpg  


  16. #16
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Quote Originally Posted by Matadem View Post
    I am going to do some tests tomorrow.
    this is not just about the square...but any other design to be cut and need some modifications.

    The main reason for this is my mach 4 pc is in the shop and my vectric pc is inside the house.
    I could redraw it in vectric with the compensation needed after measuring but going back and forward is not efficient.

    If I am already in the shop and in front of the mach 4 computer and making adjustments on the fly would be a great time saver.
    The problem is whatever Vectric software you are using most likely does not support cutter comp, your control does

    What you have been shown on how to use cutter comp most likely won't work

    Cutter comp is normally activated with a X or Y move like this snip

    G-Code G41 selects “cutter compensation left”. The tool is moved to the left of the programmed path to compensate for the diameter of the cutter.

    G-Code G42 selects “cutter compensation right”. The cutter moves to the right of the toolpath

    G-Code G40 cancels cutter compensation

    Here is some more information that may help you to get it working https://gcodetutor.com/gcode-tutoria...pensation.html

    Attached Thumbnails Attached Thumbnails Offset cutting in Mach 4 how to di this-cutter-comp-jpg  
    Mactec54


  17. #17
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Offset cutting in Mach 4 how to di this

    Matadem

    Just checked with Vectric and their software does not support cutter comp, so if you want to use cutter comp you will have to edit each program after it is posted

    In their software tool selection, you can change the tool diameter to get your part cut size you need.

    If you need parts to fit together, you could use their inlay function this will compensate so male and female parts will fit together no cutter comp needed.

    Mactec54


Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Offset cutting in Mach 4 how to di this

Offset cutting in Mach 4 how to di this