Thank you for the knowledge. I really want to get into the machining trade but I don't have any money to spend on a trade school program. I got a job at a company that produces fasteners. I'm in the heading department but I want to work my way to the cnc machine. Please keep sharing your knowledge. Thank you again.
Thank you for watching!....Same here, I started in my early 20's at a small factory and they had a couple of old CNC machines and I thought it was cool, so I keep asking if they would allow me to learn that stuff and I began to read books and understand how to program and then company allowed me the chance.......In the early 2000's the company purchased 6 HAAS machines and from there I read the manuals every night for months to understand everything....Most companies now usually have a dedicated programmer, but we didn't and we all had to learn programming ourselves at the HAAS controller with no CAD system....Good luck with your future in machining!
I know this is wrong but the way I was taught was lets say for instance you want to make a .025" Chamfer on a part that's 2" in DIA. It would be .025(Chamfer) + .016(1/64 Tool Radius) = .041 x 2(doubling it because it's per side) = .082 and thats the x value that you need to be below the final diameter. So the starting value of x is 2.0 (Final Dia) - .082 = 1.918". To calculate Z it's just .025(chamfer) + .016(Tool Radius) = .041 So the Gcode would look something like this. G00 X1.918 Z0.010 G01 Z0.0 F.002 X2.0 Z-.041 If you don't want to touch the face of the part when making a chamfer then you just need to add .02 to the equation. So to calculate X it would be .025(Chamfer) + .016(1/64 Tool Radius) + .02(compensation) = .061 x 2 = .122 And now just subtract this from your finished(or stock) diameter. 2.0 - .122 = 1.878 Keep Z the same as above and just approach the part to .020. So the Gcode would look something like this. G00 X1.878 Z0.020 G01X2.0 Z-.041 This way you don't have to start the chamfer at Z.0.0 I don't know how this works but thats the way I was taught. Seems like kind of a quick hack way to do it but I mean hey it works surprising well for me.
Campfirecrucifix…..you are correct in your method. One the you could do and I’ve done in the past is rapid to Z0. Proceed to face the part and move away from Z….say .010 and then feed up to the X compensation value that you had while moving your Z back to Z0. and then proceed from there.
Very thorough explanations. Thank you very much for all the info. Question: Do you happen to know anything about Mori Seiki CNC Lathes, and if so, how they differ from Haas CNC Lathes?
Hi there.....if you are manually programming a chamfer, you do need to know what the radius value of the insert is.....then if you are going to use a different angle, it would be helpful to have the HAAS chart to help you with your X and Z starting and ending points. In the manual, there is a section called "Tool nose compensation". The charts should be there. I found this......page 65 has the beginning of charts. www.haascnc.com/content/dam/haascnc/en/service/manual/operator/english---lathe-operator's-manual---2005.pdf
Thanks for the information! I have a question about cutter comp. If I’m facing a part from the top down at a 15 degree angle towards the z0 do I need to use a g41 or g42 to get the right angle?
Hi Ali……usually a G41 would be usually for a internal cutting ( boring path) and I personally used a G42 for all outside diameter cuts starting at X0 Z0 centerline and work my way up to the major outside diameter. I’m going to assume you might be able to use cutter comp working from the top down……for instance from a X dimension of 1.00 inch working down to X0. Does the print you are working off of give a dimension on your Z depth for your 15 degree angle?
It starts at z-0.07 inches and it goes to z0 it’s a second operation on a nylon ring that is mounted on a rubber jig that’s why its machined from the top down otherwise it will come off the jig, normally I just start above the x from the start and bring it below the x on the end the radius of the insect but I wanted to try using cutter copm
@@alielhoujairi2420 Okay, based on your starting Z-.07 location and being that its 15 degree angle, I'm assuming your part diameter is roughly just over 1/2"? I did try myself at work running both G41 and G42 and G41 seemed like it might potentially work. I did a quick program in MDI and ran it in graphics to see if it would work. So, I went Z-.125 and rapid to X.75 and proceeded to write , G01 X. 522 G41 F.005 (Your Z axis will shift in the negative direction since cutter comp is being called up, so whatever your tool radius is, it will shift that amount). G01 Z-.07 X0. Z0. X-.06(probably don't need this) Z.150 F.01 G00 Z.25 G40 (then rapid away from here) It might work for you.....good luck !
Thanks I really appreciate that info and everything you post on RU-vid really helps me since I’m a self thought machinist, I’ll try g41 the next time I run this job.
Thank you for watching!! Me personally, I like to program using cutter comp (G41 or G42). G42 is used for turning your outside diameter and G41 is used for turning your inside diameter. So when you are programing a part and lets say you want to do a .020" corner break on the outside diameter. Lets say you have a piece of stock that measures 2.125" and you are turning a part to 2.00" and want to add the .020" chamfer. I personally like to rough face and leave about .010" for a cleanup pass. I will make up a super quick program below. G00 Z.01 G00 X2.30 G01 X-.062 F.007 G00 Z.1 G01 X0. Z0. G42 F.005(cutter comp on) X1.96(subtract .04 from 2.00") X2.0 Z-.02 Z-1.0 X2.25 G00 X2.30 G40(Cutter comp cancel) With cutter comp, the machine will automatically figure out where to start the angle, based on the cutting bit radius. Just remember, whatever tool you have doing the facing and turning, be sure to have in offsets the value of the radius of the tool entered and the tool tip direction......usually that will be a 3. Hope this helps :-)
@@TimsCNC-Tractors-and-more Thanks a lot for replying. That was very quick response, I truly appreciate it. I was asking about corner breaks on chamfer or other corners to avoid sharp edges. Usually how much of a sharp corner do we give? And should it be chamfer or a fillet?
@@ijasmuhammed991 There is gonna be many variables as to how much corner breaks or fillets are allowed based on the part print. I know where I work, its usually labeled a .010" max amount for a fillet and edge breaks. So, we use a roughing cutter with a .015" radius edge insert and we leave about .020"-.030" oversize for a finish pass using another tool with an insert of either a .004" or .008" radius insert. Hope that helps :-)
Hi Sergey.....I think I understand what you’re saying, but you don’t add the radius of the cutter to your 2.0 dimension. The chart I briefly showed in the video was based on mainly what a lot of companies use for facing tools, and many of them use a .0312 radius bit insert. The calculation I came up with is based on what angle you want to cut at ( in this video it was 45 degrees) so, the compensation values will change on your starting and ending points for both the X and Z axis. If you use cutter compensation, which is a G42 code, you can write your program with the exact starting and ending points and the machine will automatically do the compensation values for you. I did make a video for that explaining how that works. I’m not sure if this helps you out, but hopefully it did ! 😃
@@TimsCNC-Tractors-and-more Hi , I got it but seems like you had have started with R compensation and finish machining without? I would like to write manually but didn't understand how create the program! Can you show again please chamfer . I know only as example : . . . G42 .G50....S.....M03 G96....S.... G0 X2.2 Z.1 G1 X... Z0. F.02 G1 Z.05 A135 F.007 ( chamfer. 05____45°) . . . M05 M09 M01; I would like understand without G42 can you show again please? Thanks
@@sergeyb6954 try watching this video of mine also explaining manual and using cutter comp. ru-vid.com/video/%D0%B2%D0%B8%D0%B4%D0%B5%D0%BE-EQvuhAG9se0.html
@@sergeyb6954 hopefully I can explain this a little bit for you. Based on what you listed in order of your G codes, you don't usually list your G42 where you have it listed. 1) The G50 code is for max spindle rpm(for example s3000 - which means 3000rpm) 2) The G96 code is surface speed(which depends on the material you're cutting). 3) G00 X2.2 Z.1(so you are doing a rapid move to X2.2 Z.1) 4) It doesn't show you doing a face cut, so I will assume a feed cut to Z.005 (just for this example) and now feed down your X axis to say X-.062 ( assuming you're using a .0312 radius insert on your facing tool.) 5) Here's where it might get tricky for you........The A135. code is a automatic chamfer call.....meaning, the machine knows that you want to do a 45 degree chamfer. If for example you wanted to do a 30 degree chamfer, that would be a A120. Now, the Z.05 would need to be a negative value to feed into the part (Z-). If you leave it as a Z.05, it will feed in front of the part. 6) If you leave the current program as listed, you could do a cutter comp move such as - G01 X0.Z0. F.007 G42 X2.0 Z-.05 A135. (just using X2.0 for example) Z-2.0(just making this up) X2.3 G00 X10.G40(Cutter comp cancel) then finish you g codes from here. -Or you could write- G01 X0. Z0. G42 F.007 X1.900(remember, everything in X is always doubled) X2.0 Z-.05 Z-2.0 X2.3 G00 X10. G40 etc,etc,etc. 7)-Now, for manual compensation- -I'm assuming you're using a .0312 radius bit- Lets say you are doing a .050" by 45 degree angle. Remember, your Z compensation is gonna be .0183 added to your Z value....So you take your .050 + .0183 and you get .0683. This is your Z- amount you need to put in your line of code where Z will end (I will show you here in a minute). Now, for you X dimension here's what you need to do----just remember, everything in X is doubled. So now, the .050 chamfer you wanna do, take the .050 and multiply by 2 and you get .100 Now, you need to add the compensation amount to that dimension. The compensation amount for the X value is .0366----so, you take .100 + .0366 =.1366 So, if you want to have you cutter come up from X0. and end up at X2.0----you would subtract .1366 from 2.0 and get 1.8634 So, you feed up to X1.8634, and the make your Z move from here. G01 X0. Z0. F.007 X1.8634 X2.0 Z-.0683 Z-2.0 (just making this up) X2.3 G00 X10. Z10.(just making this up) 8) The M05 code stops the spindle The M09 code turns off the coolant. I personally turn off the coolant after my last feed move.....but thats just me. The M01 code is a optional stop code. In order for that to work, you need to turn on optional stop at the controller. M01 acts like a M00, which stops machine motion. I really hope I didn't confuse you!!
Thank you for watching my video! Not sure if you have the HAAS Lathe manual where you work.....there is a section in the book that gives you the correct amount of compensation based on what angle you want to do and what radius insert you are using. Usually its for using a 1/64 insert radius and a 1/32 radius insert. If you don't have the manual where you work, you can go to the HAAS website and download the manual. I did another video about using cutter comp also. That uses a G42 code for O.D. turning. I personally use cutter comp ALL the time :-)
In the video, I had a X compensation value of .0366 based on a 45 degree chamfer. If you are doing a different angle, the value will change. This is based on a .031 radius insert.
