[Dakmotron]

I've just recently started programming on a HAAS ST-20 Lathe. I would like to know exactly how tool comp works on this if anyone could help that would be amazing.

When I setup my program with G41 enabled what does it do? I know it's to compensate for the tool facing left that's about all I know. When I write a program...lets say the diameter is .500 and I want to rough to .4295 when G41 is active it ends up cutting way more then it was programmed to I believe it came to .309. Now...I have the radius of the tools setup in my offsets and have everything touched off. When I run the same program with G40 enabled everything comes out how it was programmed.

So what am I missing? The person who runs another lathe (Okuma) says I should make all my programs with tool comp on but every time I do nothing comes out correctly. Does anyone have any advice or insight to my G41 problems?


Thanks in advance.

[mariojl]

Not enough data in the post.
Are you using an insert with 0.032 R?? If you're turning an OD, then should use G42, use G41 for ID. G40 cancels compensation.
By using the wrong compensating command the machine is compesating as if you're doing an ID, thus, is substracting the nose R. 4 times ( one diam. on de OD and one diam. on the ID.
Mario

[Dakmotron]

I'm using multiple inserts. One with a .032 for rough another with .016 for finish and various other things. I think my mistake was that I was using G41 to cut an OD (Which would explain the broken tools)...and I should have been using G42. If that really was my only problem...you probably saved me a huge headache for tomorrow. I thought I had read in the manual that G41 was for left cutter comp and G42 was for right cutter comp. Maybe I just misunderstood what that meant.

Sorry for such a newbie question! I've only been working in a shop for a few months and decided to try and get the other Lathe they have up and running.

Thanks for the help!

[angelw]

I'm using multiple inserts. One with a .032 for rough another with .016 for finish and various other things. I think my mistake was that I was using G41 to cut an OD (Which would explain the broken tools)...and I should have been using G42. If that really was my only problem...you probably saved me a huge headache for tomorrow. I thought I had read in the manual that G41 was for left cutter comp and G42 was for right cutter comp. Maybe I just misunderstood what that meant.

Sorry for such a newbie question! I've only been working in a shop for a few months and decided to try and get the other Lathe they have up and running.

Thanks for the help!

Whether G41 or G42 is used is determined by viewing which side of the Tool Path the tool is when viewed from where the tool started and in the direction its traveling. For example, an OD turning tool located at the back of the machine, feeding towards the chuck in the Z axis will be to the Right of the programmed tool path, therefore G42 will be used. A tool starting close to the chuck feeding towards the tail stock, will be to the Left of the tool path and therefore G41 is used.

Although you make mention of having the radius of the tool set in the Offset Page, you make no mention of setting the Imaginary Tool Tip Orientation. There is a separate column where this can be set and will be a number between and including 0 and 9, although 0 and 9 describe the same Imaginary Tool Tip Orientation. For a Right Hand OD turning tool the number used will be 3. For a forward machining Boring Bar, Imaginary Tool Tip Orientation number 2 is generally used. You will find a table of all the Imaginary Tool Tip Orientations available and their corresponding describing numbers in the HAAS programing manual.

Regards,


Bill

[Ydna]

There are specific times when it's bad to have G41/G42 active (roughing cycles for instance). But like CDC on a mill, you have to activate and deactivate G41/G42 on the lathe with a "lead in" and "lead out" move. That might be part of the problem.

Forgive me if you already know this but I'd like to point it out just in case. The lathe G41/G42 compensation is different compared to mills. What it does is compensate any diagonal or curved areas of your workpiece so the part's profile becomes aligned with the radius of the tool, instead of the theoretical programmed point of the tool. The round tool's programmed point won't touch your part if it's moving in a diagonal or arc motion. So the machine has to compensate for the round nose, or the program has to compensate for it, either way depending on how it's programmed (by hand versus CAM system).

In the end, if you're cutting a straight line motion in the Z direction to create a shaft with a set diameter, the end result diameter should be the same whether you have G41, G42, or G40 active. Same thing when cutting along the X direction, the part will be the same thickness regardless of the comp. However, as soon as you add in diagonal moves or any arc movements, that's where the tool comp will change the shape SLIGHTLY to account for the nose radius. BUT! It's probably not a huge change, dependung on the part and tools being used, but generally it's only something you'd notice when measuring it.
Because of that it makes me wonder if something else is going on if your part is different by a hundred thou in diameter, like the tool geometry offset or something...

[haastec]

Lathe programming workbook link.

http://www.egr.unlv.edu/~kevinn/CNCw...ammingBook.pdf

They use this book in some of the training classes. Hopefully it can help you out.

Good luck!