Cutter compensation..


Results 1 to 19 of 19

Thread: Cutter compensation..

  1. #1
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default Cutter compensation..

    Hello.
    New here at the forums, i will probably find the answer in some thread but i'm too lazy right now =)

    I'm using Mastercam 9.0 for my "small" home projects, with a mill using fanuc (don't remember what version) but anyways, i'm having problems when using cutter compensation (wear)..it generates too short path (imo), If using for example G41 it reads it and moves only 1mm in X and nothing in Y, i would like to make that moting a bit longer, but how?

    I'm not very familiar with the program but i have tried everyhing i can think of without any success..

    Any help would be great!
    And sorry for my bad english =)

    Similar Threads:


  2. #2
    Member
    Join Date
    Jun 2005
    Location
    us
    Posts
    232
    Downloads
    0
    Uploads
    0

    Default

    Insted of wear use control it will generate a toolpath a least the radius of the cutter.

    Tim


  3. #3
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    For V9.0, you have 2 options

    1/- extend your geometry
    2/- use "Lead in/out" , this will add additional movement to the start and endpoints of your contours , the arc is the entity the connects to your geometry , the line is the extension onto the arc along which the cutter comp. is taken up, ( or if at the end, cancelled )

    On many machines, cutter comp is taken up or cancelled on a line only
    -if you use "Wear" , then the compensation value in the control should be 0(zero) , lead in / out ( lines & arcs ) can be zero or +ive. ( you are programming the tool centreline)
    -if you use "Control" , then the compensation value in the control should be the tool radius , lead in / out ( lines & arcs ) can be zero or greater than the tool radius.( you are programming to the part contour )

    If you can get V9.1 or .2 - go for it , it has more options in the lead in / out area ( eg extend/shorten path )



  4. #4
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by driftmaster View Post
    Hello.
    New here at the forums, i will probably find the answer in some thread but i'm too lazy right now =)
    I should have come back saying, "sorry, I don't have the time, but you'll find that someone has already answered your query" LOL.

    anyway, hope the answer helps



  5. #5
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    Superman, thank you for replying =)

    I messed with lead in/ out but i'm still not satisfied..i think..First it position the tool at "X-7.502 Y1" And reads g41 moving to "G1 G41 D1 X-7.5 Y0."
    I can get 1mm in X or Y but not both, how come? =(
    Or is it ok to just read it in X or Y?
    I think i read in machine manual it must be in both X and Y in order to work right..
    Hmmf..



  6. #6
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    OK, let us go back to some sort of default settings

    use 2Dcontour,wear, left, XYoffset=0
    geometry = a straight line starting at X0Y0 to X100 Y0
    tool #1 = 16mm diameter endmill, length off#=1, dia.off#=1

    in the lead in / out dialog area
    on "lead in" side
    line tangent
    line length = 50% (8mm)
    arc length = 50% (8mm)
    arc sweep = 90 deg

    now click the arrow in the middle to copy data to "lead out" side
    accept and re-generate t/path , now post this t/path
    it should be similar to the following
    Code:
    G0 X-8. Y24. ( rapid to point )( start of lead in line)
    G1 Z0.
    G41 D1 X-8 Y16 ( lead in line- takeup comp.)
    G3 X0. Y8. R8. ( lead in arc )
    G1 X100. ( the actual geometry )
    G3 X108. Y16. R8. ( lead out arc )
    G40 G1 Y24. ( lead out line - cancel comp. )
    G0 Z3. ( retract )
    If line length has a setting of zero, this line will not be output
    If either arc length or arc sweep has a setting of zero, the arc will not be output

    A line by itself can only be "perpendicular" or tangent", if you want a line at a 45 deg approach, it is controlled by the arc sweep and the line will be tangent

    ie tangent, line 55mm,arc 13mm,sweep 30deg ( try it )
    now change tangent to perpendicular, then try a 90 deg sweep

    this should all be viewable on the screen, your post may have some issues and we are trying to understand lead in / out at this stage

    Your query "I think i read in machine manual it must be in both X and Y in order to work right.. "
    Depends on your machine, compensation movement has a look ahead function ( it would be better explained in your machine's manual )

    a rough example

    a straight line from X0Y0 to X100 and taking up comp
    Code:
    X-20. Y0.    ( if D1 in control =8.0)
    G1 G41 D1 X0.( goes to X0 Y8)( comp ON)
    X100.        ( goes to X100 Y8)
    G40 X120.Y0  ( goes to X120 Y0)(comp OFF)




  7. #7
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Superman View Post
    OK, let us go back to some sort of default settings

    use 2Dcontour,wear, left, XYoffset=0
    geometry = a straight line starting at X0Y0 to X100 Y0
    tool #1 = 16mm diameter endmill, length off#=1, dia.off#=1

    in the lead in / out dialog area
    on "lead in" side
    line tangent
    line length = 50% (8mm)
    arc length = 50% (8mm)
    arc sweep = 90 deg

    now click the arrow in the middle to copy data to "lead out" side
    accept and re-generate t/path , now post this t/path
    it should be similar to the following
    Code:
    G0 X-8. Y24. ( rapid to point )( start of lead in line)
    G1 Z0.
    G41 D1 X-8 Y16 ( lead in line- takeup comp.)
    G3 X0. Y8. R8. ( lead in arc )
    G1 X100. ( the actual geometry )
    G3 X108. Y16. R8. ( lead out arc )
    G40 G1 Y24. ( lead out line - cancel comp. )
    G0 Z3. ( retract )
    If line length has a setting of zero, this line will not be output
    If either arc length or arc sweep has a setting of zero, the arc will not be output

    A line by itself can only be "perpendicular" or tangent", if you want a line at a 45 deg approach, it is controlled by the arc sweep and the line will be tangent

    ie tangent, line 55mm,arc 13mm,sweep 30deg ( try it )
    now change tangent to perpendicular, then try a 90 deg sweep

    this should all be viewable on the screen, your post may have some issues and we are trying to understand lead in / out at this stage

    Your query "I think i read in machine manual it must be in both X and Y in order to work right.. "
    Depends on your machine, compensation movement has a look ahead function ( it would be better explained in your machine's manual )

    a rough example

    a straight line from X0Y0 to X100 and taking up comp
    Code:
    X-20. Y0.    ( if D1 in control =8.0)
    G1 G41 D1 X0.( goes to X0 Y8)( comp ON)
    X100.        ( goes to X100 Y8)
    G40 X120.Y0  ( goes to X120 Y0)(comp OFF)
    Thank you!
    That made it!
    Now the lead in and lead out is just like i wanted..

    Thanks alot mate!



  8. #8
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Great!!

    I tried to give examples of what you can do by just altering the lead in / outs
    Many create extra geometry, just to get the tool to drop in on a safe spot,
    some times creating extra goem. is unavoidable, but I try keeping that option for the more difficult paths.

    Steve



  9. #9
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default x3

    Hello again..

    I have been trying X3 for a while now, now been trying to work out the cutter compensation again and got in to problems..

    So Superman, or somebody else who is familiar with Mastercam..Help needed =)

    Ok, so i'm trying to make a simple circle with cutter compensation inside the countour.

    Withour lead in or lead out it posts :

    "N40 G0 G90 G54 X14.978 Y1.M3 T225
    N80 G43 H5 Z25.
    N100 G1 G41 D0 X14.975 Y0.
    N110 G0 Z5.
    N120 G1 Z-34.
    N130 G3 X-14.975 R14.975
    N140 X14.975 R14.975
    N150 G0
    N160 G0 Z25.
    N170 X14.975 Y0.
    N180 G40 X13.975"

    Here i can see last line is not like it used in mc9.0, it used to move in both X and Y while reading G40..Hmm, meaby its enough in X? don't know, havent tried in machine yet.

    Not i try with lead in and lead out as i want to have more movement in G41 movement, now just 0.003 in X axis. (i got a alarm while ago because it didnt have enough movement..hmm)

    Now it posts :
    "N40 G0 G90 G54 X6.268 Y-12.021M3 T225
    N80 G43 H5 Z25.
    N100 G1 G41 D0 X6.975 Y-11.314
    N110 G0 Z5.
    N120 G1 Z-34.
    N130 X12.632 Y-5.657
    N140 G3 X14.975 Y0. R8.
    N150 X-14.975 R14.975
    N160 X14.975 R14.975
    N170 X12.632 Y5.657 R8.
    N190 G0
    N200 G0 Z25.
    N210 X-10000. "

    So now im happy with the G41 movement but something is messed with the lead out part i think...What should i change or tweak?

    I used the tool in mastercam x3 to upgrade my post processor from v9.0 to x3..

    //



  10. #10
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    N40 G0 G90 G54 X6.268 Y-12.021M3 T225
    N80 G43 H5 Z25.
    N100 G1 G41 D0 X6.975 Y-11.314
    N110 G0 Z5.
    N120 G1 Z-34.
    N130 X12.632 Y-5.657
    N140 G3 X14.975 Y0. R8.
    N150 X-14.975 R14.975
    N160 X14.975 R14.975
    N170 X12.632 Y5.657 R8.
    N190 G0
    N200 G0 Z25.
    N210 X-10000.

    N100 is a move to the start of lead in with cuttercomp using offset#0 ( most use the same # as the tool # for length and dia offsets )
    (H0 and D0 usually are zero and are not changeable )
    it then rapids down to the clearance plane, feeds into the job (note!! no feedrate applied - should be XY Feedrare on the G41 line , and Plunge rate on the Z)
    N140 and N170 are your arc lead in/outs
    you seem o be missings the lead out line and a cutter comp cancel (G40), without this you may get errors going to the next point

    We have set our order of doing profiles as:-
    -set co-ord system
    -rapid to start point ( usually 1st point of lead in line )
    -set spindle RPM , start spindle
    -rapid descent to clearance plane and take up tool length offset
    -coolant on
    -Rapid to Retract plane
    -feed to Z depth
    -take up comp ( onto the 2nd point of lead in line )
    -lead in arc ( if required )
    -do profile
    -lead out out ( if required )
    -lead out line, cancel comp on last point
    -rapid retract or do next depth ( depends on your settings )

    Our Okuma's require a line to take up and cancel comp on



  11. #11
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    First, thanks alot Superman for taking your time and replys.

    Now lets see, Feedrates are posted as should be, it was just that i didnt bother put any there because im just testing. But i tried, and its like it should.

    Same with the D0, it was specified in tools and i changed it. Posts it like it should.

    So ive been messing more with the lead out settings and it just wont work. posts the damn x-10000 everytime...

    In v9.0 i havent seen this happen..

    If i try to not use the EXIT in lead in/ lead out it posts
    N160 G40 X-14.975 R14.975

    But im not satiesfied with this neather..=(

    Why won't it just make a simple move in x and y like it does when it reads the G41 code?

    I had no issues in mc9.0 after your help..

    Is this a error in post processor or what do you think?
    I have no experience working with post processors...



  12. #12
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    OK, you're working with V9
    can you make a test Mcam file with a circle and a line
    and create operations to profile both using what you think is correct lead in and out ( so it looks good on screen )
    -create a ZIP folder and place this Mcam file and the post you're using
    -attach this ZIP folder to your next posting so I can have a look

    Your on a FANUC machine , 3 axis ?
    I think the X-1000 is set in the post , but I'll have a look first for you
    I should be able to compare it to one of our V9 posts

    Steve



  13. #13
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    Hey again.

    Well, i was working with V.9.0. But now im trying to learn X3 instead.
    Post processor is working like i want with v9.0, but with X3 cutter compensation is a mess.

    I used the post update thing in X3 but something is wrong with the post i think..
    You will see when you try posting program =)

    I made a test file for you to take a look at.Also included posted programs in both v9.0 and X3, here you can see what goes wrong..
    Same lead/lead out in v9.0 and X3..

    The machine is a Horizontal Mori with Fanuc control..



    Quote Originally Posted by Superman View Post
    OK, you're working with V9
    can you make a test Mcam file with a circle and a line
    and create operations to profile both using what you think is correct lead in and out ( so it looks good on screen )
    -create a ZIP folder and place this Mcam file and the post you're using
    -attach this ZIP folder to your next posting so I can have a look

    Your on a FANUC machine , 3 axis ?
    I think the X-1000 is set in the post , but I'll have a look first for you
    I should be able to compare it to one of our V9 posts

    Steve


    Attached Files Attached Files


  14. #14
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default Hello

    Hello "Superman"

    Have you had any time over to check what could be causing the problem?

    Have a nice day



  15. #15
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Had a look at your X3 stuff.

    before modifying the post, have a look at the control settings for your machine, cutter comp section where comp is cancelled after retracting from the operation. This may solve a couple of your problems.

    on the top toolbar <settings> <edit machine def.> <edit control>
    this opens a dialog for this machines defaults, files, posting targets, etc. , one of the items is that cutter comp.
    have a look at those settings

    This is probably also the area that is controlling your X-1000 . For this can also come from the "Misc. Intergers", "Home Position" or "Reference Point" buttons, we'll look closer after getting comp running OK


    Your output using comp is a little strange, it does not follow exactly what is happening on-screen, and if comp is cancelled after retracting, and you have a large comp value then the point that the tool goes to before retracting is not the point on-screen. This can be a situation causing an un-explained crunch.

    Also look carefully at your lead-outs if you have one that puts the tool into the contour, sometimes it will omit the lead-out and also miss putting in the G40 (eg doing an inside circle and the lead-out is a tangent line instead of perpendicular line - tool will stop on the end of the contour and retract there )


    Your post is a little different to mine in the area of cutter comp
    Does your machine take-up and cancel comp on arcs ?
    or does it need a line for comp to work ?
    Fanucs and Okumas need lines, I've got my post to output a warning if comps start or finish with an arc



  16. #16
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    Heya there.

    Thanks for checking in out and taking your time..

    I have been messing with the "machine & control def" with to sucess at all =(..Hmm, i will try more, but close to giving up now..

    Machine i'm using cant take up cutter comp. in arcs.
    It's just like you said, a line thats needed..

    Yeah, i'm aware of the problem when typing large comp value..
    But hey, that's what im used to not the best way but it works..

    Just gotta get the damn thing to post the right stuff.
    Im pretty sure something goes wrong when updating the post from v9.0 to x3, just dont know what..



  17. #17
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default hmmm

    Superman.

    I've been messing with the settings and so on for a couple of days now..
    I just don't get it to work..
    Don't know what to change in the post, it's all too confusing for my brain =).

    Would be great if you could have a look at it once again and see if you can find the problem..
    Sorry for being such a pain



  18. #18
    Flies Fast Superman's Avatar
    Join Date
    Dec 2008
    Location
    Antarctica
    Posts
    3110
    Downloads
    0
    Uploads
    0

    Default

    Had a closer look a the post header you put up for the X3 example

    This post was originally set-up for V7 (1999= last mod date ) and has quite a few mods up to X2, especially in the cutter comp area. The mods also make it a bit harder to follow. Look for "ppost$" near the post end as an indication

    There are also changes to variable names that can create problems after X2.

    You may be getting a post upgraded each time, which is not all bad, but you may be losing a lot of functionallity that is available in X3, you are actually limited by the age of your post.

    Do you have a reseller that could do a current post for you ?
    You can also download the MpmasterX3 post from IHS(-link) and actually compare the outputs in the comp area. I think you would be more happier with a new post version instead of an old one dressed up.



  19. #19
    Registered
    Join Date
    Apr 2009
    Location
    Sweden
    Posts
    30
    Downloads
    0
    Uploads
    0

    Default

    Hmm, thats worse then i thought then..
    But hey, thanks for having a look at it atleast.

    I could use the "generic fanuc" post if i just got couple of things added to it. But i guess that's adding custom stuff in the post too..=(
    I would like to have the look-a-head function added so its read in when tool is changed (g8 p1)and g8 p0 before next tool is changed..
    And also m11, b0, m10 on all look changes too..

    Ofcourse this would be no problems for reseller, but they are damn pricey and im a cheap bastard =)

    But thanks anyway!!



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

Cutter compensation..

Cutter compensation..