Setup alignment

[JPMach]

Just to piss you off all I do is clamp the part anywhere on the table, bring my reinshaw probe down and touch two points, measure the angle and then G50 coordinate rotaion to the angle I want and I'm done!

JP

[JPMach]

I meant G68
sorry

JP

[ozzie34231]

Yes. At the time I started this thread I was not aware of the ability of my controller, Mach 3, to to rotate the axis in the xy plane. I've since learned that it is a way to mostly accomplish what I needed.
In Mach 3 the rotation won't enable jogging in the new axis only along the standard xy. It does enable machining and MDI movements. That being the case, I'm not sure how to "touch off" after the axis have been rotated. I'll need to think about that some more. How do you do it JP?

Jerry

[JPMach]

I have a 2005 Haas Vf-4 with probing option, I just bring the ruby tip of the renishaw probe down and run a macro program from renishaw to measure the angle, which I can then read and adjust with G68(very useful for vises, no onger do I have to align vises, just probe and go). No I can't jog at the angle that the G68 invokes but it rotates the program to that. The posistion readout actually changes such that a commanded move of X3. actually shows up as more or less depending on what angle was put in the G68 line.

JP

[ozzie34231]

Okay I understand that.

But if the origin of the part does not lie along the line of the two points that were used to rotate the machining axis, how do you manuever to that 0,0 point if you can't jog there.

Well, ,,,,as I'm writing this I'm beginning to think it doesn't matter. If I jog to that point in any manner and then referance it as 0,0 and the controller takes that to mean 0,0 in the rotated axis, it works. I'll have to try it.

Jerry

[lerman]

The ability to do coordinate transformation is one of the things I hope to add to EMC when I get around to it.

Ken

[JPMach]

Some of the renishaw Macros that came with the machine ( I had to call renishaw to get a book to understand how to use them, like 80 page long book) are for finding corners or centers of webs. The corner find macro can take up to 4 hits, two on each side of the corner.To find the corner of a block that is on the table at 45 deg for instanece all I have to do is call up that macro and tell it how far apart to take the hits and press cycle start. Because of the great angle the probe might move to take a hit but after a certaion distance it faults out saying that the part is not there, this just requires one more varible to be put into the macro to open up the tolerance for how far to move before faulting. Once it takes the four hits I know where the corner is and at what angle it is rotated and can then use that variable with that G68 command (All of which can be put at the begining of a program and it can do while I walk away).

I did a test once, put a vise on the table at about a 45 deg angle then clamped a piece of alum in the vise and did the corner find and roated the axis to part and made a cut in x only about 6" long. I then measured the part for paralelism and it was right on the nuts!

Round work is almost as easy, For putting keyways in large shafts I just lay the shaft in the tslot of table, clamp it and tell the probe that it is a web and because it goes to the same depth to on each side of the shaft it finds the center of the shaft. When it is done measuring it moves to the center automatically, where I then take a hit in Z to find the top, look in machinery's handbook calculate total depth of cut and the keyway is put to right depth the first time every time.

JP

[JPMach]

I just looked the book I got from renishaw through email is actually 224 pages long!
It gets deep at points but most is easy to understand. What sucks is that Haas doesn't even tell you about them, they give some probe cycles through visual quick code but they are very basic. I saw all of these macros on the machine and asked haas how to use them and they said I would have to call renishaw.

JP

[Geof]

Originally Posted by JPMach I saw all of these macros on the machine and asked haas how to use them and they said I would have to call renishaw. JP

Did you ask the applications people at Haas or the technicians at your Haas dealer?

[JPMach]

Both, they mostly said just to use the quick code provided or if I wanted to figure out the advanced stuff myself to ask renishaw.

JP