Cutter compensation for groove-turning operations
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 41
  1. #1
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default Cutter compensation for groove-turning operations

    Hello PM community,

    I am looking for any suggestions or feedback on groove-turning applications and cutter compensation. These applications use multi-purpose parting tools that are also designed for OD profiling, and even facing. Iscar and Thinbit are popular among companies who make these tools.

    Here's an example of a Thinbit tool in action:



    I realize that many people would hand program something like this, but that is not an option - we have to use Mastercam. A major point of confusion has been the cutter-compensation. Since we are using both sides of the tool, we are essentially toggling between G41 and G42, and also using at least two quadrants: 3 and 4. Generating a tool-path is not the issue - the confusion comes from setting up the tool at the controller (Fanuc).

    Is anyone familiar with these operations?

    How did you setup your offsets at the controller?

    Did your toolpath toggle between G41 and G42?

    Did you have to enter the quadrants in your offsets (usually a T value)?

    Sice we are using two quadrants, did you have to use two offsets for the same tool at the controller?

    Thank you so much

  2. #2
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,322
    Post Thanks / Like
    Likes (Given)
    1962
    Likes (Received)
    840

    Default

    I typically will touch the front of the tool for T0101, then touch the rear of the tool for the opposite offset.
    That offset would be something like T0120 (tool 1, offset # 20, or whatever you like)
    Since the tool (in my case) is a standard Iscar top grip or similar, the tool tip direction is 8. ( a standard OD grooving tool)

    Yes, my program will rough out the groove, finish with a G42, then the opposite side with a G41.


    I have no clue how to do that in mastercam, as I don't run it.

    ***Since you are using a cam system, why do you need more than 1 offset?
    M/C should be able to program off the center of the tool, or wherever you want.
    The program probably won't even call for a G41 or G42, as the program does all the trig for you, and spits out G1/G2/G3 moves.

    In OneCnc lathe, you can opt for offsets (G41/G42) or have the program trig it out, and not use TNR.

    Doug.

  3. #3
    Join Date
    Nov 2013
    Location
    north of Bean town
    Posts
    487
    Post Thanks / Like
    Likes (Given)
    79
    Likes (Received)
    160

    Default

    Quote Originally Posted by doug925 View Post
    I typically will touch the front of the tool for T0101, then touch the rear of the tool for the opposite offset.
    That offset would be something like T0120 (tool 1, offset # 20, or whatever you like)
    Since the tool (in my case) is a standard Iscar top grip or similar, the tool tip direction is 8. ( a standard OD grooving tool)

    Yes, my program will rough out the groove, finish with a G42, then the opposite side with a G41.


    I have no clue how to do that in mastercam, as I don't run it.

    ***Since you are using a cam system, why do you need more than 1 offset?
    M/C should be able to program off the center of the tool, or wherever you want.
    The program probably won't even call for a G41 or G42, as the program does all the trig for you, and spits out G1/G2/G3 moves.

    In OneCnc lathe, you can opt for offsets (G41/G42) or have the program trig it out, and not use TNR.

    Doug.
    this is correct. Mastercam will figure out the tool width offset and program accordingly. just make sure the operator touches off the correct side of the tool

  4. Likes Fancuku liked this post
  5. #4
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,969
    Post Thanks / Like
    Likes (Given)
    353
    Likes (Received)
    1967

    Default

    I usually cringe when I hear that we HAVE TO USE this or that tool, but ...

    Yes, I do as Doug mentioned and pick up the tool twice with 2 offsets.
    The only exception is that I use dir 3 for the front of the tool and dir 4 for the back edge for two reasons.
    First, when the operator looks at the offset page it is immediately obvious which side of the tool is used.
    Second, for dir 8, normally the center of the tool radius is picked up as Z0, which means that it must be used comped or otherwise programmed.

  6. Likes doug925 liked this post
  7. #5
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,674
    Post Thanks / Like
    Likes (Given)
    384
    Likes (Received)
    756

    Default

    Why do you need cutter comp? - just let the cam program calculate the path based on the tool width and corner radius- you're not going to comp the tool anyway are you? Are you controlling the radius of your part that closely? Probably not.

  8. Likes doug925 liked this post
  9. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,969
    Post Thanks / Like
    Likes (Given)
    353
    Likes (Received)
    1967

    Default

    Quote Originally Posted by Dan from Oakland View Post
    Why do you need cutter comp? - just let the cam program calculate the path based on the tool width and corner radius- you're not going to comp the tool anyway are you? Are you controlling the radius of your part that closely? Probably not.

    Dan
    If you need to control the profile of the groove, then it would be an absolute nightmare to have to re-post every time just to get within tolerance.

    I'd say 80% of my grooves ( on the B/P ) are controlled to +/-.001 on dia, typically +/-.002 on width and .005 total on internal radii and outside edge break.
    Add in the occasional positive or negative side drafts which are also +/- 2.0 degree .....

  10. Likes mayu liked this post
  11. #7
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    133
    Post Thanks / Like
    Likes (Given)
    330
    Likes (Received)
    42

    Default

    I wouldn't mess with cutter comp with groove tools. Just have Mastercam trig it out for you.

  12. #8
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,908
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1580

    Default

    Quote Originally Posted by Fancuku View Post
    I wouldn't mess with cutter comp with groove tools. Just have Mastercam trig it out for you.
    Hello Fancuku,
    Yes, I agree. However, using a Tool Offset for the Leading and Trailing edge of the tool, as suggested earlier by Doug, is good practice if the both sides of the groove have tight position tolerance. Without the two offset, its irrelevant whether Tool Radius Comp is used or not, as TNR Comp won't enable you to move one side of the groove only. Two offsets allows each side (Leading and Trailing) to be moved independent to the other.

    Regards,

    Bill

  13. #9
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    133
    Post Thanks / Like
    Likes (Given)
    330
    Likes (Received)
    42

    Default

    You are making things more complicated in my opinion. And if you use G41/42 in the wrong direction you will be screwed. You'll cut more than you needed too.

  14. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,908
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1580

    Default

    Quote Originally Posted by Fancuku View Post
    You are making things more complicated in my opinion. And if you use G41/42 in the wrong direction you will be screwed. You'll cut more than you needed too.
    I agreed with you in my previous Post with regards to using Tool Radius Compensation. Having an Offset for both sides of the tool doesn't equate to using TNR Comp. But good luck if you want to move one side of a groove without affecting the other, if you only have an offset for one side of the Tool.

    The alternative to the two Offsets is to fudge the program. And as the tool wears, you can continue to fudge the program and hope that you, or the button pusher, doesn't fuck up with editing the numbers. Or you could just change an Offset value. I know what I'd rather do.

  15. Likes Dan from Oakland liked this post
  16. #11
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,917
    Post Thanks / Like
    Likes (Given)
    1390
    Likes (Received)
    1589

    Default

    Featurecam has specific functionality to use separate offsets for each side of a grooving tool, MC have that also?

    I use it sometimes, sometimes I just use a single offset and tool width. I'll choose depending on the part and the operator. I've once or twice had trouble with operators putting an x wear offset on to bring the diameter in but forgetting to apply it to both offsets, then standing scratching their head trying to figure out why it's not doing what they expected.

  17. #12
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    Quote Originally Posted by doug925 View Post
    Why you are using a cam system, why do you need more than 1 offset?
    Hi doug925,

    The short answer is for control. We get parts with extremely tight tolerance OD groove-profiles with odd angles, radii, and steps. The sides of these profiles are often dimensioned from the center of a groove in both directions. Having a separate offset allows us to control these dimensions separately in either direction. These dimensions are often as tight as .01 mm.

  18. #13
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    Quote Originally Posted by SeymourDumore View Post
    I usually cringe when I hear that we HAVE TO USE this or that tool
    Hi SeymourDumore,

    I sympathize with your perspective, but we are trying to get away from hand programming. For small shops or simple programs it is okay, but for complex production work, it is an accident waiting to happen. When changes occur, such as tool numbers (sharing a machine with multiple jobs), work offsets, or moving the program to a different machine, someone has to edit the program manually, which leads to typos. I can give you a million scenarios, like when a the customer tells us to change an radius or an angle from 37.5 degrees to 38.6 degrees, and the programmer has to make these changes by hand.

    With CAM we can fully utilize the power of simulations, create tool libraries for each machine that have correct feeds and speeds, build templates for repeat jobs, create stellar CAD illustrations, and share this information with our clients via the cloud. Welcome to 2020!

  19. #14
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    Quote Originally Posted by gregormarwick View Post
    Featurecam has specific functionality to use separate offsets for each side of a grooving tool, MC have that also?
    Hi gregormarwick,

    Yes my initial thoughts were to rough the profiles with the plunge turn feature, and then finish the profiles by manipulating Mastercam's finish groove offset parameters. My primary concerns are the tool quadrant values (t value), which nobody commented on. I'm not entirely clear on this, which was one of my main reasons for posting. I was more-or-less brainstorming, trying to understand as many perspectives or methods as possible.

  20. #15
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    Quote Originally Posted by Fancuku View Post
    You are making things more complicated in my opinion. And if you use G41/42 in the wrong direction you will be screwed. You'll cut more than you needed too.
    What's more complex is having only one offset to control +/- .01mm dimensions of a complex OD groove profile, which are called out from the center of the profile outward in both directions. G41 and G42 allow us to control these dimensions separately in either direction. You only need to call the cutter-comp on the finish passes. The cutter-comp moves are generated by the CAM program to avoid typos.

  21. #16
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,908
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1580

    Default

    Quote Originally Posted by mayu View Post
    G41 and G42 allow us to control these dimensions separately in either direction.
    Not necessarily. I assume from your Previous Post in this Thread, that you're using a different Imaginary Tool Type Number for the Leading and Trailing edges of the Insert, and therefore, an Offset for the Leading Edge and a second Offset for the Trailing Edge. It's the two Offsets that gives you the control of both sides of the Groove, not G41/G42 per se.

    If you were to calculate the Tool Path based on the Radius of the insert being used, two offsets, without the use of TNR Comp (G41/G42), would suffice.

    Regards,

    Bill

  22. #17
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    California
    Posts
    19
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    [QUOTE=angelw;3538040It's the two Offsets that gives you the control of both sides of the Groove, not G41/G42 per se.[/QUOTE]

    Yes you're right - that is another way of doing it. There's always more than one way to do things. We've chosen to use cutter-comp because it's easier to read the programs as they will be generated to print. In addition, the cutter-comp doesn't confine us to the same insert. The cutter comp only needs to be used on the final finish passes, so it's not that complex.

    I appreciate your technical, non-emotional, feedback. I was simply trying to reach out to anyone who has tried this approach. My primary concern was in regards to the t quadrant settings, which nobody bothered to answer.

  23. #18
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,908
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1580

    Default

    Quote Originally Posted by mayu View Post
    Yes you're right - that is another way of doing it. There's always more than one way to do things. We've chosen to use cutter-comp because it's easier to read the programs as they will be generated to print. In addition, the cutter-comp doesn't confine us to the same insert. The cutter comp only needs to be used on the final finish passes, so it's not that complex.

    I appreciate your technical, non-emotional, feedback. I was simply trying to reach out to anyone who has tried this approach. My primary concern was in regards to the t quadrant settings, which nobody bothered to answer.
    Hello mayu,
    Its not another way of doing it, its the way you're doing it, only you're using TNR Comp with the two Offsets and its the two Offsets that makes it work.

    With regards to the "quadrant", I assume you mean the Imaginary Tool Type, it's somewhat irrelevant. Practically any tool type number will work, so long as the Tool is set to correspond with the Tool Type number used; the control will work it out. However, for the sake of logic, Tool Type 3,4, or 8 would be used for an OD Turning operation.

    Regards,

    Bill

  24. Likes doug925 liked this post
  25. #19
    Join Date
    Nov 2002
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    3,322
    Post Thanks / Like
    Likes (Given)
    1962
    Likes (Received)
    840

    Default

    Quote Originally Posted by angelw View Post
    With regards to the "quadrant", I assume you mean the Imaginary Tool Type, it's somewhat irrelevant. Practically any tool type number will work, so long as the Tool is set to correspond with the Tool Type number used; the control will work it out. However, for the sake of logic, Tool Type 3,4, or 8 would be used for an OD Turning operation.

    Regards,

    Bill
    This is what I assumed the OP meant. (Tool tip direction) If quadrant is something else entirely, then I have no clue.


    @ Seymore

    You are right. The use of a tip direction of 3 & 4 is a better option.

    Doug.

  26. #20
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    210
    Post Thanks / Like
    Likes (Given)
    59
    Likes (Received)
    46

    Default

    Quote Originally Posted by mayu View Post
    Hello PM community,

    I realize that many people would hand program something like this, but that is not an option - we have to use Mastercam.
    Maybe you should be thankful your employer provides you with great tools others go without?

    pebcak.jpg

  27. Likes CNC Hacker, doug925 liked this post

Tags for this Thread

Bookmarks

Posting Permissions

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