Programming a G71 canned cycle - HAAS CNC Lathe for beginners / Intermediate
Вставка
- Опубліковано 15 вер 2024
- Welcome to my videos on hopefully being able to teach beginners who have never programmed a CNC machine. I myself programmed HAAS CNC Lathes for over 15 years and I started from scratch not knowing anything about writing codes!! (Aggghhh!!) I had to manually write new programs at the machine controller and that's kind of what these videos are about. Most places now probably have a dedicated person for writing programs and drawing blueprints...but, If you are just starting out and need to learn how to program by hand, I hope these videos will help :-)
In this video, I explain how to program a G71 canned cycle. A G71 is a stock removal canned cycle that I used all the time in programming. I know this video is kind of long, but I wanted to make sure I explained it clearly :-) Hopefully it will make sense after you watch me ramble on....ha!!
I realize this may be a more advanced video for beginners....but, I still figured it could help out.
Please be sure to check out my playlist of my other CNC videos!!
• HAAS CNC Lathe - Learn...
Awesome job explaining learned a lot in this short video
That’s awesome!! Thank you for the kind words 😎🤘
Could you please do some more videos on canned cycles for lathe, I have learned so much from your videos. Awesome video by the way you really explain things so I can understand. Thanks for the videos!
Thank you so much for the very kind words!! I do plan on doing updated videos, and I will make a note to do more videos with canned cycles.
İt would be awesome.we will be appriciated.Thanx for your efford
Thanks you Sir
Thank you for watching!!
Can a use a G96 in a G71 cycle? Im working on a diameter of .110 to .375 thousands. Its making a lot of shatter... It has S1800 F.002 its A2 steel...
Hi there…….So yes, you can place a G96 surface speed while doing G71.
Your G96 will be placed before your G71 cycle.
Here’s the tricky part……there are many variables that could be giving you chatter on your finish.
Tool nose radius being used.
Length of part being turned
Finish pass in program might need adjustment
So, it could be many variables.
You mentioned S1800….is this your max rpm in your program?
I’ve worked with A2 also. It can be tricky trying to get a nice finish.
If you can let me know as to how long your part being turned…..maybe I could give you more ideas.
Your two,s and Z look the same. I had to make sure. In the beginning i thought i was watching the wrong video because i coudnt find the Z.
Yeah, sorry about the handwriting being a little sloppy and thank you for watching it!
Using g71 canned cycle type two with cutter comp g40 where do I compensate apparently the machine doesn’t like the comp because it can’t switch tool nose directions
Hey there….thanks for the question.
I’m currently at work and just wanted to send you a quick video link from HAAS talking about this.
ua-cam.com/video/0_GiMspK0pc/v-deo.htmlsi=NF4Mm2pgEGnsa4bI
This video is very useful, thanks 👍👍👍
Thank you for watching!!
Amazing, thanks for the awesome video!
Thank you for watching!
Thank you
Thank you for watching!!
First off, THANK YOU for taking the time to explaine all this! You make it so simple for someone starting off without any experience in tool and die!
I have been working more and more with our CNC machines, but I am burning through carbide inserts on my boring bar. The culprit is a backside chamfer on an ID (or so I think). The program has the boring bar plunge into the DOM after it finishes removing the inside material, and it causes the tips to break often. Do you have any suggestions on what could help extend the life of my tips?
Hi Tim, thank you so much for the kind words and watching my video!...Well, there are many variables here so I'm gonna ask you a few questions first.
(1) What kind of material are you machining? (2) What is the diameter of the bore you are doing? (3) Did someone else write the program? (4) Are you on a HAAS Lathe? (5) Are you doing a G71 canned cycle? (6) I assume there is a drilled hole that goes through the part? Sorry for all the questions.
If you want to, write down the G codes you are using and the canned cycle that is being used. If you are using a G71 canned cycle, make sure that the U value in the canned cycle is a negative value(-). So you would have a code like this,
G71 P#Q# U-.02 W.005 D.05 F.005
So, you would enter in the P the line # to where to begin....say line # 10.....so that would be P10.
Now, what line number do we end at....let's say line 13.....that would be Q13.
Now, lets say you are doing a 2" bore and you drilled a 1" hole through the part. Lets say you are doing a Z depth of 2" deep. Here's a quick example of setting up a boring path I usually did,
N8 G00 X.950 Z.100
N9 G71 P10 Q13 U-.02 W.005 D.05 F.005
N10 G00 X2.00 Z.06
N11 G01 Z-2.00
N12 G01 X.980
N13 G00 X.950
N14 M09
N15 G00 X10. Z10.00 M05
Etc, etc, there is soooooooo much more I could include, but let me know how your program is written first before I get to far ahead of myself...haha!!
@@TimsCNC-Tractors-and-more The material is 1026 DOM, It is initially 1.750" and is bored out to 1.781" on our HAAS ST-30 Y. With the size of the bore we are taking the stock off in one pass, no drill. The program is generated by MasterCAM right now, but I have been going back and adjusting some of the issues that I have noticed. I believe the programmer isn't double checking the parameters to adjust the feedrate when the boring bar makes the plunge for the back chamfer.
@@murderface3131 Ohhhhhhhh....gotcha. First off, Nice machine! I begged my former employer to get a Y axis lathe! Haha!! I personally never used Mastercam, I programmed everything myself. A place I just began working at uses Mastercam and yes, I scroll through the program and notice some feedrates are WAAAAY to fast, in my opinion.
I would check that feed rate when it's making that plunge in the back of the part to make the chamfer. If your going through insert bits and the tips are breaking, that would be my first guess.
@@TimsCNC-Tractors-and-more If I was going to alter that feedrate, would it just be adding a (F) code at the end of the line that does the plunge?
@Timothy Buchanan Yes, the f code is the feed rate code. Sometimes the even use an E code for feed rate, but very rarely. Whats the feed rate now? Try lowering the number....if you have a feed rate of F.010 - try cutting it in half....F.005
I’ve been trying to run a g71 cycle on a haas st10 but I keep getting an alarm that says (370 canned cycle geometry error) and I went through the user’s manual and still couldn’t figure out why I’m getting this message
Yeah, sometimes the smallest error will generate an alarm code. If you want to show me how you wrote your program starting at your G71 block and where you end....maybe I can help out.
I know I should’ve ended the g71 cycle at n16 instead of n17 but the reason I did it this way because when I wrote a g70 finish cycle I had to end it at n17 so It can read the g40 because I got a message saying that I needed to have a g40 in the program, so what I want to know is can I use different P and Q numbers in g71 and g70 for the same cut?
@@alielhoujairi2420 I'm not sure if you attached your program to this post, because I don't see it.
I would need to see your programmed path in order to hopefully help you out.
Usually whatever your P & Q codes are in the G71 cycle will need to be the same in a G70 cycle. I'm assuming you are using cutter comp in your machining cycle?
One thing I always do is to make sure your starting X location and your ending X location are the same. I will write a small program below turning a make believe 1.00" part using cutter comp and using a .031 tool radius....I will illustrate below with line #'s -
N1 T101 (turn o.d.)
N2 G50 S2000
N3 M97 S500 M03
N4 G54 G00 Z0.01 G96 S500
N5 X1. M8
N6 G01 X-.065 (allow for tool radius) F.01
N7 G00 X1.1 Z.1 (notice X & Z value)
N8 G71 P9 Q15 U.02 W.01 D.06 F.01
N9 G00 X-.065 Z.07
N10 G01 G42 X0. Z0. F.01
(cutter comp on)
N11 X.95 F.005
N12 X1.0 Z-.025 (chamfer)
N13 Z-1.0
N14 X1.08 F.01
N15 G00 X1.1 G40
(notice X value on line 15 - Cutter comp is also turned off)
N16 M09
N17 (G00 X and Z home or ?)
N18 T100 (tool cancel)
N19
N20 T202 (Finish turn o.d.)
N21 G50 S2000
N22 M97 S500 M03
N23 G54 G00 Z0.1 G96 S500
N24 G00 X1. 1 M8
N25 G70 P9 Q15
N26 M09
N27 (G00 X and Z home or ?)
N28 T200 (tool cancel)
(etc, etc)
Now , this example is if you are using a different tool to do a finish pass......you could use tool 1 for a finish pass if you wanted to......you would just put your G70 P9 Q15 line right before the M09 line. Also notice the feed rates being used in G71 cycle......the feed rate listed on the the G71 line is the feed rate being used to remove material......when you do your G70 cycle, the feed rates listed in the programmed path will now be used .
Hopefully this makes sense ! :-)
If you are using a different tool for the finish pass do you rapid the tool into the starting position and then apply the the g70 code?
Patrick, I personally do that. So the spot you rapid too for beginning the roughing cycle, I use the same spot to rapid for beginning the finish pass.
will the canned cycle also repeat m code if its in the code like for opening and closing a steadyrest or clamp type follow rest on a shaft?
Thank you for the question! I think I understand what you are asking......I don't believe you can have a M code for opening and closing of a tailstock rest or a tailstock opening and closing of a sub clamp included in the canned cycle.
Did you try writing your M code move in the canned cycle and watch it graphics mode to see if you get an alarm?
I know that some programs I wrote in the past, such as turning a piece of bar stock, I would do a canned cycle to remove as much material as possible and after that canned cycle finished, I would get the turret out of the way and program a tailstock move with a live center to engage the part...(should be a M21 code). From there I would continue with a finish pass...which is a G70 code to follow your values you wrote in your G71 canned cycle.
If you are doing a large piece of stock and are removing material in stages, you will need to write multiple canned G71 cycles....For example, lets say you start at the front of the part and write your first G71 canned cycle. Now, lets say your P and Q codes are P10 and Q20 (for this example). You go ahead and machine that section and now you finish that section and want to move on and machine the next section. Stop the machine and move the turret away and do your clamping that you mentioned about. From here, if you wanna do more material removal and want to incorporate another G71 code for stock removal, you are gonna have to use different P and Q values. Now you can write your new G71 stock removal cycle and for this example you could use a P30 and Q40.
Just remember, for each G71 stock removal cycle you program, you need different P and Q codes. Be sure to watch the program in graphics mode and see its doing what you want it to do and also it checks for alarms in your programming format.
I hope this helps!
Why would you not go into a g70 cycle to have a nice clean up pass?
Hi Steve.....you are absolutely correct...I always run a finish pass and in the video at the 2:30 part, I mention the use of a G70 finish pass using a different tool, but this demonstration was mainly focused on doing a G71 stock removal when you are first starting out.
@@TimsCNC-Tractors-and-more ok, no problem there. I do really like your videos. Wish they were around 20 years ago.
@@stevebriggs9135 .....Thank you for the kind words.
I wish UA-cam was around 20 years ago !! 😆😆
what about the retract value ? where do we mention that
Hi There!....Do you mean sending the machine home? I didn't show that in this video....I only mentioned in the video that you would continue your writing to send your X and Z values home. I ran out of chalkboard in the video (Ha!!).
So, after your done machining your G71 canned cycle(in this video it was N12 Q20....which is line 12 to line 20)....I usually program my X axis to head home , and then my Z axis home.
@@TimsCNC-Tractors-and-more no i mean in the G71 cycle how do you know how much the tool is going to retract like after the depth of cut like how much the tool is going to move in x and z positive direction
@@AmanDeep-ki3xf Gotcha....so, I'm going to make sure of my answer when I go back to work on tomorrow. I'm pretty sure the X axis retract is usually the amount of your depth of cut per pass, and the Z axis usually goes back to your original Z starting plane before the G71 was called up.
I will reply back again in a day to confirm my answer.
@@AmanDeep-ki3xf…..I wrote a mock program to verify and yes….the D value you have in the G71 line is the retract value in X and the Z retracted to the original Z starting plane just before you call up G71.
@@TimsCNC-Tractors-and-more love it 👍🏻thanks for clearing up my doubt 🫡