G71 I parameter What is it?


Results 1 to 9 of 9

Thread: G71 I parameter What is it?

  1. #1
    Registered pepsis's Avatar
    Join Date
    Jan 2015
    Location
    20292
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default G71 I parameter What is it?

    Ok, i recently started working as machinist. I am familiar with mechanical engineering...now my boss wants me to learn fixed cycles for turning.

    One of the first few is of course G71. Now our unit is of older ones. At least it look older to me. It is some VICTOR lathe and an "older" fanuc 15T i suppose. I read documentation today. it supports type I sigle block G71 and here is example of program block:

    N5 G72 P6 Q11 U0.04 W0.2 I1.0 K1.0 D7000 F0.3

    Here are "explanations":

    I - distance and direction of rough finishing along x axis (delta i) in radius programing in the finishing cycle
    K - distance and direction of rough FINISHING along the z axis (delta k) in the rough finish cycle

    While at the same time it says:

    U - distance and direction of finish allowance along the x axis in dia programing (in radius it is U/2 )
    W - distance and direction of rough of finish allowance along x axis (delta w)


    You see my doubting here, right. In that example which is following this text (i gave it here in reverse order), it says clearly that some are for DIAMETER programming, and some are for RADIUS programming. Then it states that some alloances are for finishing (and we all know what finishing means, right?), and some are for "ROUGH FINISHING" is this suppose to be SEMI finishing?!

    So is that what I and K are for? Or am i missing something here. How else thy could be in same block???

    Do they stay for type II controls too???

    TNX in advance!

    Similar Threads:


  2. #2
    Registered
    Join Date
    Dec 2011
    Location
    USA
    Posts
    34
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    I cant answer that, but i only use P Q U W D F no I or K.This has worked fine for me for years.Id like to know when they would come in handy though.



  3. #3
    Registered pepsis's Avatar
    Join Date
    Jan 2015
    Location
    20292
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by MetalCarpenter View Post
    I cant answer that, but i only use P Q U W D F no I or K.This has worked fine for me for years.Id like to know when they would come in handy though.
    I know, right? I mean, every single example i have found on the net, doesn't include I or K. Thus my non understanding of what they are really used for. I can just assume that they are something like semifinishing (rough finishing), but what i have learned this little time working is that i should never just jump to conclusions like that. That is why i ask here.

    (I don't want to ask my boss, 'cause even if he does know, i want to look good. Looking good (not physically ) mean better pay in the end. )



  4. #4
    Member
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1227
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by pepsis View Post
    Ok, i recently started working as machinist. I am familiar with mechanical engineering...now my boss wants me to learn fixed cycles for turning.

    One of the first few is of course G71. Now our unit is of older ones. At least it look older to me. It is some VICTOR lathe and an "older" fanuc 15T i suppose. I read documentation today. it supports type I sigle block G71 and here is example of program block:

    N5 G72 P6 Q11 U0.04 W0.2 I1.0 K1.0 D7000 F0.3

    Here are "explanations":

    I - distance and direction of rough finishing along x axis (delta i) in radius programing in the finishing cycle
    K - distance and direction of rough FINISHING along the z axis (delta k) in the rough finish cycle

    While at the same time it says:

    U - distance and direction of finish allowance along the x axis in dia programing (in radius it is U/2 )
    W - distance and direction of rough of finish allowance along x axis (delta w)


    You see my doubting here, right. In that example which is following this text (i gave it here in reverse order), it says clearly that some are for DIAMETER programming, and some are for RADIUS programming. Then it states that some alloances are for finishing (and we all know what finishing means, right?), and some are for "ROUGH FINISHING" is this suppose to be SEMI finishing?!

    So is that what I and K are for? Or am i missing something here. How else thy could be in same block???

    Do they stay for type II controls too???

    TNX in advance!
    Hello pepsis,
    I and K is used to specify a Semi Finish margin in addition to the Finish Allowance specified by U and W. When using G71 Type 1, with I and K values specified, rough cuttings occurs parallel to the Z axis leaving a margin specified by I and K, followed by a pass following the profile shape leaving any finish allowance specified by U and W.

    I and K are also available with G71 Type II, FS15 format. When using G71 Type 2, with I and K specified, the tool returns to the Start Position after the Roughing cuts have been completed, then performs a pass following the profile shape leaving any finish allowance specified by U and W.

    Regards,

    Bill



  5. #5
    Registered pepsis's Avatar
    Join Date
    Jan 2015
    Location
    20292
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by angelw View Post
    Hello pepsis,
    I and K is used to specify a Semi Finish margin in addition to the Finish Allowance specified by U and W. When using G71 Type 1, with I and K values specified, rough cuttings occurs parallel to the Z axis leaving a margin specified by I and K, followed by a pass following the profile shape leaving any finish allowance specified by U and W.

    I and K are also available with G71 Type II, FS15 format. When using G71 Type 2, with I and K specified, the tool returns to the Start Position after the Roughing cuts have been completed, then performs a pass following the profile shape leaving any finish allowance specified by U and W.

    Regards,

    Bill

    THANKS A MILLION, Bill! You assured me now, for i was in doubt.

    Do you happen to know, why D (thickness of cut) is this format of four digits. I assume in my example (it is in metric units btw) that this depth of cut is 0.3mm, and it is given in example by D3000. Or is it 3 thousands of mm, but that would be too little. even for finishing cut.

    Here is the code again so you don't have to go back and search:

    N5 G71 P6 Q12 U0.4 W0.2 (I1.0 K1.0) (added brackets since we never actually use these two) D3000 F0.3 (here is what my shop considers very heavy feed)

    And here is one in imperial from CNC Handbook


    N8 G71 P9 Q16 U0.04 W0.004 D1000 (again, D to be thou of an inch too small, a whole inch...impossible, right?) F0.1 (not so big of feed in inches, right).


    So what's the deal with D? I just came back from work, i didn't have much time since last night to take a look, but i just realized that i don't understand that one as well. I wathced some videos on you tube, but this is something every presenter just assumes that the one who is watching is familiar with... beginners are not. I know, of course what feed and speed and CSS is.

    I mostly work with metric, but since a lot of literature is in imperial units, i try to understand them as well.



  6. #6
    Member
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1227
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by pepsis View Post
    THANKS A MILLION, Bill! You assured me now, for i was in doubt.

    Do you happen to know, why D (thickness of cut) is this format of four digits. I assume in my example (it is in metric units btw) that this depth of cut is 0.3mm, and it is given in example by D3000. Or is it 3 thousands of mm, but that would be too little. even for finishing cut.

    Here is the code again so you don't have to go back and search:

    N5 G71 P6 Q12 U0.4 W0.2 (I1.0 K1.0) (added brackets since we never actually use these two) D3000 F0.3 (here is what my shop considers very heavy feed)

    And here is one in imperial from CNC Handbook


    N8 G71 P9 Q16 U0.04 W0.004 D1000 (again, D to be thou of an inch too small, a whole inch...impossible, right?) F0.1 (not so big of feed in inches, right).


    So what's the deal with D? I just came back from work, i didn't have much time since last night to take a look, but i just realized that i don't understand that one as well. I wathced some videos on you tube, but this is something every presenter just assumes that the one who is watching is familiar with... beginners are not. I know, of course what feed and speed and CSS is.

    I mostly work with metric, but since a lot of literature is in imperial units, i try to understand them as well.
    Hi pepsis,
    There are some addresses that have to be specified without a period and are expressed in units of least programmable increments. There is no particular reason for this, its just the way it is.

    Given that the unit for D is the least programmable increment, the default parameter setting for a control set in Metric Mode will be 0.001mm and in Imperial Mode 0.0001 inches. Accordingly, D3000 in Metric Mode will be 3000 microns, or 3.0mm and D1000 in Imperial Mode will be 1000 one-ten thousandths of an inch, or 0.1 inches.

    Regards,

    Bill



  7. #7
    Registered pepsis's Avatar
    Join Date
    Jan 2015
    Location
    20292
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by angelw View Post
    Hi pepsis,
    There are some addresses that have to be specified without a period and are expressed in units of least programmable increments. There is no particular reason for this, its just the way it is.

    Given that the unit for D is the least programmable increment, the default parameter setting for a control set in Metric Mode will be 0.001mm and in Imperial Mode 0.0001 inches. Accordingly, D3000 in Metric Mode will be 3000 microns, or 3.0mm and D1000 in Imperial Mode will be 1000 one-ten thousandths of an inch, or 0.1 inches.

    Regards,

    Bill
    Right. I saw this in handbook. Isn't this a lot. 3mm in metric and 0.1 inch (2.54 mm). Do i have to program it this big? Can i just leave out leading zeros and type D300 (like 300 microns)? I'm sorry if I am bothering you, but you seem to know these things. Guys that program at work, don't have a clue why something is like it is. They just know they HAVE to do something in certain way, and that's it. I want to know all my options, and if i can find out what every option can do. I am not satisfied with knowing stuff half way. So sorry again.



  8. #8
    Member
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1227
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by pepsis View Post
    Right. I saw this in handbook. Isn't this a lot. 3mm in metric and 0.1 inch (2.54 mm). Do i have to program it this big? Can i just leave out leading zeros and type D300 (like 300 microns)? I'm sorry if I am bothering you, but you seem to know these things. Guys that program at work, don't have a clue why something is like it is. They just know they HAVE to do something in certain way, and that's it. I want to know all my options, and if i can find out what every option can do. I am not satisfied with knowing stuff half way. So sorry again.
    The depth of cut, "D", will depend on size, rigidity of the machine and workpiece and the horsepower available. 3mm isn't that big a cut; I've often programmed Turning Centres to take 6mm (radius value) and greater depth of cut. You're not compelled to program any particular Depth Of Cut, As a general rule, the depth of cut will be whatever the machine, workpiece and tooling will handle. To answer your question directly regarding the D address, if you want to use a 0.3mm depth of cut you would just program D300.

    Regards,

    Bill



  9. #9
    Registered pepsis's Avatar
    Join Date
    Jan 2015
    Location
    20292
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: G71 I parameter What is it?

    Quote Originally Posted by angelw View Post
    The depth of cut, "D", will depend on size, rigidity of the machine and workpiece and the horsepower available. 3mm isn't that big a cut; I've often programmed Turning Centres to take 6mm (radius value) and greater depth of cut. You're not compelled to program any particular Depth Of Cut, As a general rule, the depth of cut will be whatever the machine, workpiece and tooling will handle. To answer your question directly regarding the D address, if you want to use a 0.3mm depth of cut you would just program D300.

    Regards,

    Bill
    You Sir deserve a drink, right F...N NOW! You do drink, right? Ok, you don't have to say anything. But that deadly combo of one burbon, one scotch one beer is on me, if we ever meet eyes to eyes. Of course, domestic finest plum brandy we make here (me and my gran dad ).

    Few years back, there was and advert here (before i went to study) that through some immigration organization people from Serbia could apply for work at sheep farms in AUS, and one of rewards was some kind of limited citizenship. But conditions were that you couldn't leave country for five years. If you did, you could still come back and work, but would never get a citizenship. I suppose they figured if you couldn't be still there for that amount of time, you don't want it. Any way, my gran dad said to me, that if don't want to go and study, we can start our own farm. Which we did anyway. More of an "urban" kind of farm. It is not in city, it is not in the middle of nowhere...

    Any way if you ever come to Serbia, come to me. I'll get you that drink.

    Now, about that G71. Is there a short answer, how to deal with complex contour when none of machines don't support type II. They can only handle type I of G71. Do i program "roughly" the contour with out complex grooves, and then after that program some other tool, and do conventional coordinate-to-coordinate tool path, with all the little things, like number of passes and everything? This should be my last Q on the topic



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

G71 I parameter What is it?

G71 I parameter What is it?

G71 I parameter What is it?