Camsoft cutter comp


Results 1 to 1 of 1

Thread: Camsoft cutter comp

  1. #1
    Registered
    Join Date
    Sep 2012
    Location
    Canada
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Camsoft cutter comp

    Hello.
    I have an OKK MCV 630 that has had a Camsoft retrofit put on it (by the previous owner)
    I cannot figure out how to get cutter comp to work (G41 and G42).
    I have tried calling up the tool # in the line prior to the comp line and it does nothing.
    I have tried putting the tool # in the comp line and it does nothing.
    I am using tool #1 and that is where I have the comp value loaded as well (on the tool screen in Camsoft). So my tool length and comp value are in the same address (T01)
    Does Camsoft require the tool length compensation and cutter comp value to be entered as 2 seperate adresses, T01 for tool length and T41 for comp value as an example?



  2. #2
    Registered
    Join Date
    Dec 2009
    Location
    USA
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Camsoft cutter comp

    When you do a T01 to select a tool #1 on Camsoft Pro, it selects the tool height on line 1 in the tool settings menu. There is no provision for say T0121 where you can set a tool height from a different line. That's the easy one, so I hope that is working for you. Just Txx and the height is set.

    For Tool Comp, though, it may be a bit more confusing. First off, make sure you completely understand how tool comp is supposed to work on normal CNC machines. It is confusing enough on it's own that most people that have difficulty with tool comp are simply failing to understand how to correctly perform the first move (the compensation move). Once you are sure you understand that, check C:\AS3000\CNC\GCODE.FIL for the G41 and G42 commands. You should see something like the following:

    TOOLCOMP OFF
    -----G40
    TOOLCOMP LEFT
    -----G41
    TOOLCOMP RIGHT
    -----G42

    This is the default for a 3 axis CNC machine for example. If yours is different, then someone programmed your machine to work differently. But I don't think there is much someone would program differently.

    Anyway, When I execute a G41 or G42, I use the following method:

    T3 M06 (TOOL 3)
    M08
    G17 G90
    G54
    G00 Xxxx Yxxx S4000 M03
    Z.5
    G01 Z.2 F1.2 (FOR THIS EXAMPLE, I AM NOW BELOW MY CUTTING PLANE OFF THE EDGE OF MY PART)
    G42 D3 Xxxx (OFFSET 3 - FIRST CUTTING MOVE Xxxx MOVES INTO MY PART - THIS IS THE COMPENSATION MOVE)
    G01 .... (THIS MOVE IS NOW FULLY COMPENSATED)
    ...
    G01 ....
    G40 Xxxx (TURN OFF COMPENSATION - Xxxx IS THE TURN OFF COMPENSATION MOVE)
    G01 .... (UNCOMPENSATED MOVE)

    But there are a couple things wrong with this as I have had difficulty with it as well - probably my own fault. First, the D3 on the G42 line is ignored I believe. I left it there because my post processor came that way, but I don't think it matters according to the docs for Camsoft Pro. The Camsoft docs say to just do a G41 or G42 and that will enable compensation using the compensation value of the currently selected tool. You still have to do the compensation move (i.e. the first move after G41/G42 is not compensated, but instead is the move that enables compensation - this is the norm for all CNC machines). The Xxxx in my G42 line causes the first move (the "compensation move" that moves the tool into compensation). All following moves are compensated.

    But I have not had good results fully compensating my tools, so I only compensate for wear in Camsoft, and I let my CAM program do the tool comp. Meaning, if T3 is a 1/2 inch end mill, and I try to compensate the full 1/4" inch radius plus wear, I sometimes get weird results. So if my 1/2 inch tool is actually 0.498 inch, I will compensate for the 0.002" error in Camsoft, but I will use Computer Compensation in my CAM program (the CAM program calculates the 1/4" radius comp, and Camsoft only calculates the 0.002" wear comp). With this, I have had no problems.

    To be clear, the comp problems I have encountered are probably my failure to understand how to use Camsoft tool comp, but I just decided to let my CAM program deal with it as I have more important things to do unfortunately.

    To set up wear comp in Camsoft and tool comp using Computer Comp I follow these notes - which I had to write down to make sure I didn't get confused. This is using Mastercam, but other CAM programs should have a similar capability.

    Summary of how to do Wear Compensation using Mastercam and Camsoft
    Set tool dia. to 0 in Camsoft tool menu.
    Set tool diameter correctly in Mastercam of course.
    Set Wear to -(tool wear) in Camsoft menu. (e.g. -0.002 for a tool that is 0.002" too small, ,not 0.002).
    Use Mastercam Reverse Wear, not Wear, for compensation.
    e.g. 1/2" tool, but it is really 0.400" because it has been reground.
    Wear is 0.100. (0.500 - 0.400 = 0.100)
    Set Wear to -0.100 in Camsoft tool wear field.
    Enable Reverse Wear in Mastercam and tool diameter set to 0.500".
    Tool will be driven 0.200" from the edge we want to cut.
    That is:
    Mastercam drives tool to 0.250 from edge (radius of 0.500 tool)
    Reverse Wear in Mastercam results in a G42 (instead of G41) for climb cut, which moves tool in
    reverse direction by 0.050 because it is compensating to the right side of the 0.250 line
    Mastercam directed.
    Hence, tool is -0.250 from line + 0.050 = 0.200

    Not quite what you were asking for, but maybe it will help you understand a few things and get where you want to be. Hopefully someone else will come in and explain better how to get reliable compensation for full tool radius.

    BTW, when I say I have had problems with Camsoft and tool compensation, it is more a matter of how I like to enable tool comp. I often use tool comp inside small holes where I may not have enough room to move the tool a full radius to enable tool comp. So Camsoft gives an error because my "enable tool comp" move wasn't correct. This is likely true with many (most??) CNC machines. But Mastercam can perform tool comp with a move that is less than the tool radius, so it works for me and that's why I use it. I have also had cases where I didn't get an error from Camsoft, and the tool plunged into the side of the hole ruining the part and/or breaking the tool. So to avoid possible mistakes due to my misuse of tool comp. I just use the reverse wear method.



  3. #3
    Member Karl_T's Avatar
    Join Date
    Mar 2004
    Location
    Dassel.MN
    Posts
    1542
    Downloads
    2
    Uploads
    0

    Default Re: Camsoft cutter comp

    may be repeating lohmeyer somewhat.

    Comp works off tool diameter in the tool table, must be defined there BEFORE loading your program.

    I find you need two G01 moves at a right angles to bring cutter comp in. As its cutting air on the first move, I make it at least the tool diameter. I know the first move can not be G0. Not sure its a Camsoft rule, but I could not get G02/G03 to work on the second move.

    Try this, let me know if it works for you:

    set T1 in tool table to 0.5 (1/2 inch cutter)
    T1
    G0 Y-1 X0
    G42
    G01 Y0 F10
    G01 X1
    G01 Y1
    G01 X2
    G01 Y2

    Does that work?

    Last edited by Karl_T; 10-29-2016 at 08:14 AM.


  4. #4
    Registered
    Join Date
    Sep 2012
    Location
    Canada
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Camsoft cutter comp

    Thanks for the help guys. I am going to go try it right now.
    I do understand how cutter comp works as I use it on my other machines regularly, I just can't get it on the Camsoft setup.
    I always program the profile as the cutter diameter and only compensate for wear as Lohmeyer suggested, so that should not be a problem.
    I will try your suggestions and let you know how it works.
    Thanks.



  5. #5
    Registered
    Join Date
    Sep 2012
    Location
    Canada
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Camsoft cutter comp

    I tried the way that was suggested.
    I put in the cutter dia in the tool settings. 1.00 dia for my 1" tool.
    When I initialize the program it gives me an error that says the cutter is too big.
    I program the machine on an offline cam system (Bobcad) and I always let the cam software do the initial cutter offset. I tell Bobcad I am using a 1" dia tool so it makes the path accordingly.
    So I put in 0 dia for my tool and the program will run fine, but will not add the cutter comp.
    I put the tool dia at .010 and ran the program and it ran without the 'tool too big' error, but did not put on cutter comp.
    I have put in 2 G01 moves prior to my machining moves as suggested, but no comp is added.
    I have checked in the AS3000 file as suggested and comp is turned on.
    I am not familiar with AS3000, but I think it is only the cam program. I do not use it so I don't believe any of the settings in there should affect my program execution. Is this correct?
    The program that I am trying to run is to interpolate a bore using a 1" dia tool. Cutter comp is a necessity so that I can adjust my bore size easily as the tool wears.
    This is my code. I am running 2 vises, so I have a G54 and a G55.


    (T01 1.0 DIA MILL 1)

    G00 G17 G20 G80 G90
    T01
    G54
    G00 X.185 Y0. S2400 M03
    N04 Z.25
    N05 G01 Z.1 F50.
    N06 G41
    G01 X1.0 Y.1 F50
    G01 X.335 Y0
    G01 Z.05
    N07 G17 G03 Z.02 I-.335 J0. F50.
    N08 Z-.01 I-.335 J0.
    N09 Z-.04 I-.335 J0.
    N10 Z-.07 I-.335 J0.
    N11 Z-.1 I-.335 J0.
    N12 Z-.13 I-.335 J0.
    N13 Z-.16 I-.335 J0.
    N14 Z-.19 I-.335 J0.
    N15 Z-.22 I-.335 J0.
    N16 Z-.25 I-.335 J0.
    N17 Z-.28 I-.335 J0.
    N18 Z-.31 I-.335 J0.
    N19 Z-.34 I-.335 J0.
    N20 Z-.37 I-.335 J0.
    N21 Z-.4 I-.335 J0.
    N22 Z-.43 I-.335 J0.
    N23 Z-.46 I-.335 J0.
    N24 Z-.49 I-.335 J0.
    N25 Z-.52 I-.335 J0.
    N26 Z-.55 I-.335 J0.
    N27 Z-.58 I-.335 J0.
    N28 Z-.61 I-.335 J0.
    N29 Z-.64 I-.335 J0.
    N30 Z-.67 I-.335 J0.
    N31 Z-.7 I-.335 J0.
    N32 Z-.73 I-.335 J0.
    N33 Z-.76 I-.335 J0.
    N34 Z-.79 I-.335 J0.
    N35 Z-.82 I-.335 J0.
    N36 Z-.85 I-.335 J0.
    N37 Z-.88 I-.335 J0.
    N38 Z-.91 I-.335 J0.
    N39 Z-.94 I-.335 J0.
    N40 Z-.97 I-.335 J0.
    N41 Z-1. I-.335 J0.
    N42 Z-1.03 I-.335 J0.
    N43 Z-1.06 I-.335 J0.
    N44 Z-1.09 I-.335 J0.
    N45 X-.1675 Y.2901 Z-1.1 I-.335 J0.
    N46 X.335 Y0. I.1675 J-.2901
    N47 X-.1675 Y.2901 I-.335 J0.
    N48 G01 X-.0925 Y.1602
    G40 X0 Y0
    N49 G00 Z5

    T01
    G55
    G00 X.185 Y0
    N04 Z.25
    N05 G01 Z.1 F50.
    N06 G41
    G01 X1.0 Y.1 F50
    G01 X.335 Y0
    G01 Z.05
    N07 G17 G03 Z.02 I-.335 J0. F50.
    N08 Z-.01 I-.335 J0.
    N09 Z-.04 I-.335 J0.
    N10 Z-.07 I-.335 J0.
    N11 Z-.1 I-.335 J0.
    N12 Z-.13 I-.335 J0.
    N13 Z-.16 I-.335 J0.
    N14 Z-.19 I-.335 J0.
    N15 Z-.22 I-.335 J0.
    N16 Z-.25 I-.335 J0.
    N17 Z-.28 I-.335 J0.
    N18 Z-.31 I-.335 J0.
    N19 Z-.34 I-.335 J0.
    N20 Z-.37 I-.335 J0.
    N21 Z-.4 I-.335 J0.
    N22 Z-.43 I-.335 J0.
    N23 Z-.46 I-.335 J0.
    N24 Z-.49 I-.335 J0.
    N25 Z-.52 I-.335 J0.
    N26 Z-.55 I-.335 J0.
    N27 Z-.58 I-.335 J0.
    N28 Z-.61 I-.335 J0.
    N29 Z-.64 I-.335 J0.
    N30 Z-.67 I-.335 J0.
    N31 Z-.7 I-.335 J0.
    N32 Z-.73 I-.335 J0.
    N33 Z-.76 I-.335 J0.
    N34 Z-.79 I-.335 J0.
    N35 Z-.82 I-.335 J0.
    N36 Z-.85 I-.335 J0.
    N37 Z-.88 I-.335 J0.
    N38 Z-.91 I-.335 J0.
    N39 Z-.94 I-.335 J0.
    N40 Z-.97 I-.335 J0.
    N41 Z-1. I-.335 J0.
    N42 Z-1.03 I-.335 J0.
    N43 Z-1.06 I-.335 J0.
    N44 Z-1.09 I-.335 J0.
    N45 X-.1675 Y.2901 Z-1.1 I-.335 J0.
    N46 X.335 Y0. I.1675 J-.2901
    N47 X-.1675 Y.2901 I-.335 J0.
    N48 G01 X-.0925 Y.1602
    G40 X0 Y0
    N49 G00 Z8
    Y10
    N52 M30

    Any advice would be greatly appreciated.



  6. #6
    Member Karl_T's Avatar
    Join Date
    Mar 2004
    Location
    Dassel.MN
    Posts
    1542
    Downloads
    2
    Uploads
    0

    Default Re: Camsoft cutter comp

    N06 G41
    G01 X1.0 Y.1 F50
    G01 X.335 Y0

    Not positive, but I've always made these two at a right angle. what happens when you change Y0 to Y.1 on the last line above?

    did my real simple example fail too?

    Karl



  7. #7
    Member Karl_T's Avatar
    Join Date
    Mar 2004
    Location
    Dassel.MN
    Posts
    1542
    Downloads
    2
    Uploads
    0

    Default Re: Camsoft cutter comp

    Here, I read the manual for you. First perpendicular start is required. Try these examples.

    Karl





    Tool Comp Rules and Good Standard Practices

    Here are a few places to review in order to learn more about tool comp.

    (1) Question Nos. 166, 167, 180 and 218.
    (2) TOOL COMP logic command.
    (3) FANUC manual.
    (4) Do Tutorial 8 in the AS3000 manual.
    (5) Do a search on the words Tool, Comp and/or G41 using Search for Solutions.


    Tool Compensation Examples

    (TOOL COMP EXAMPLE OF CURVE LEAD IN)
    (TOOL 1 IS .5 DIAMETER)
    (INCREMENTAL ARC CENTERS)
    M6 T1
    G90 S1200 M3
    G00 X-.5 Y0 Z.5
    G01 Z0 F30
    G41
    G01 Y-.5
    G03 X0 Y0 I0 J.5
    G01 Y1
    X2
    Y-1
    X0
    Y0
    G03 X-.5 Y.5 I-.5 J0
    G40
    G01 Y0
    G00 Z.5 M5
    M2





    (TOOL COMP EXAMPLE OF PERPENDICULAR LEAD IN)
    (TOOL 1 IS .5 DIAMETER)
    M6 T1
    G90 S1200 M3
    G00 X-.5 Y-.5 Z.5
    G01 Z0 F30
    G41
    G01 X0
    G01 Y1
    X2
    Y-1
    X0
    Y.5
    G40
    G01 X-.5
    G00 Z.5 M5
    M2


    (PROPER OUTSIDE CIRCLE CLOCKWISE)
    G90
    T1
    G01 X0Y-20 F1000
    G41
    G01 X20
    G01 Y0
    G02 X20 Y0 I220 J0
    G01 Y20
    G40
    G01 X0



    Tool Comp for Outside Circle


    (PROPER OUTSIDE CIRCLE COUNTER-CLOCKWISE)
    G90
    T1
    G01 X0Y20 F1000
    G42
    G01 X20
    G01 Y0
    G03 X20 Y0 I220 J0
    G01 Y-20
    G40
    G01 X0



    (PROPER INSIDE CIRCLE CLOCKWISE)
    G90
    T1
    G01 X30Y0 F100
    G42
    G01 X20Y0
    G02 X20 Y0 I220 J0
    G40
    G01 X30 Y0



    Tool Comp for Inside Circle


    (PROPER INSIDE CIRCLE COUNTER-CLOCKWISE)
    G90
    T1
    G01 X30Y0 F100
    G41
    G01 X20Y0
    G03 X20 Y0 I220 J0
    G40
    G01 X30 Y0



  8. #8
    Registered
    Join Date
    Dec 2009
    Location
    USA
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Camsoft cutter comp

    Re: C:\AS3000 - Yes, this is the program folder for AS3000 which is Camsoft's CAM program. You don't need to worry about that. But C:\AS3000\CNC is where you find all the .FIL files (e.g. GCODE.FIL) which determine how your CNC controller works. When you run the Camsoft Settings program, for example, or when you save tool data, it is saved in C:\AS3000\CNC.


    Re: using 1" tool to interpolate a hole and wanting to get the exact wear for accuracy.

    Yes, this is why I use wear on Camsoft, but I let the CAM program handle the tool offset most the time like you are. So CAM handles that it is a 1" tool, and Camsoft handles the -0.002" difference (e.g. a 0.998" tool) of the actual tool diameter. Read through my comments above again carefully and make sure you pay attention to positive or negative values in the Camsoft tool table. So as you discovered, to do Wear only offsets, set the tool diameter to 0 in Camsoft, and set the wear number to a negative number. Then use reverse wear in your CAM program. So for a 1 inch tool that is actually 0.998", you tell BobCAM that it is a 1" tool. You tell Camsoft that the tool dia. is 0 and the wear is -0.002. If your CAM software supports reverse wear then it will issue a G42 for climb cutting a hole and the tool offset will work because the wear is a negative number.

    I forget why I had to use reverse wear. I believe if you use normal wear (not reverse wear), then you could set the wear as 0.002 (positive) and your CAM software would issue a G41 instead of G42 for climb cutting a hole. But there was a reason I ended up having to use reverse wear. Or maybe I just decided to do it that way because I wanted the wear number in Camsoft to be negative for tools that are undersize. Regardless, play with it using obviously large wear numbers like 0.250 with a 1" tool) and you'll be able to determine what is correct for you.

    Also, because it is so easy to mess this stuff up, when I interpolate a hole like that, I plunge the tool centered in the hole, and then issue a G01 move with the G41/G42 to move the tool sideways. This normally moves the tool at least 1/4 to 1/2 of a diameter, which should be enough to properly engage tool comp using wear or reverse wear comp. Then issue a G02/G03 to arc the tool onto the cutting surface (the lead in). I only use the G41/G42 comp cut on the final pass. No point in using tool comp on the roughing cuts unless the tool you are using is a regrind and significantly smaller than the intended dia. (e.g. a 1" endmill but reground to 0.900" perhaps). Then I G02/G03 off the cutting surface (Lead out), and issue the G40 with a G01 move back to the hole center. Of course, my CAM program does all this for me - I just specify the options such as lead in, lead out, and enter on a center point. By starting the tool dead center in the hole and doing a G01, I make sure I never run into issues with cutter comp - it is so easy to get cutter comp issues if you don't.

    I didn't study your example well enough to see if you are doing this, but I see you are using a G01 for the first move. So maybe reverify you are sure cutter comp isn't working. I mean, exaggerate the wear numbers to the point you can see the tool move one way or the other of the intended cutting line and figure out what is or isn't working. If you aren't seeing any compensation from G41/G42, then look at your GCODE.FIL as I mentioned in my first post to make sure it is programmed correctly.

    Not sure I'm being helpful. Cutter comp is just one of those things you need to play with sometimes to figure out how to get it right, even when you know what you are doing. On Camsoft, I saw several cases where G41/G42 moves that worked perfectly all day long on a Haas, failed on Camsoft. Obviously I failed to understand exactly how Camsoft wants to see it work. My solution was to just use reverse wear and now it works perfect every time. But I had to play with this for a few hours to figure it out and make sure it was right.



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

Camsoft cutter comp

Camsoft cutter comp