5-axis tool setup

[cdlenterprises]

I'm new to 5-axis machining and I need to know if there is a special way to touch off tools for cutting a 5-axis profile. I've tried touching them off like a standard tool but when I tilt the head and cut a profile my depths are way off! It's a Cincinnati V5-2000 with a Siemens 2100 control. Any suggestions?

[HuFlungDung]

Are we allowed to guess?

I would imagine that reference plane for the tool setting should be at the axis of rotation for the 5th axis. Now this could be difficult to find through trial and error. Would there be a machine specification for the distance from the spindle nose to the axis of rotation?

If so, then perhaps using a tool presetter would be in order, to find how far the tool tip is from the spindle nose. This would give you a series of relative offsets for all the tools. If the tooltip reaches so far as the axis of rotation, then its length offset would be zero, if shorter, its offset could be positive, if longer, its offset could be negative, or vice versa.

[Geof]

In the Haas manual I found mention of G141 3D+ Cutter Compensation and G143 5-Axis Tool Length Compensation which somehow figure out the head tilt correction (or something).

Perhaps your manual has something similar.

[blowmebigtime]

Hi there,, I am not familiar with the Seimens control but i can tell you how I do it.. First I enter my tool dia. and radius in the tool table, ( .500 ball/.25 rad.) then I run the tool at machining rpm thru a lazer, that gives the control the length from the CENTER of the radius to to back of the HSK holder. Then for the Z height I set it off of the back of the work piece always, for example set of the table and enter .250 in the Z ( for the center of the ball). The control I run has a function called RTCP which stands for rotation tool center point,, that way for programming you don't care how long the tool is because the control backs up the radius amount. If you don't program using the RTCP then you must know the tool length before you can post you program..

[CNCRim]

You can just touch off like normal 3-axis work. But with 5-axis continous you can't put the part where every you want, it must be at the location where the program said or else. I think that is what happen in your case.

[fiveaxs]

you have to use g141 for 5 axis continuous contouring. This is the only way the control can track the datum and tip of tool during rotation.

[flick]

There is a five axis Haas where I work. I wasn't aware that the Haas control was capable of doing the offset compensation, but from reading the above posts, it appears that it can. The other method (what we do) is to tell MasterCAM the incremental distance in X and Z from our G54 to the B axis center of rotation. It assumes that the A axis center of rotation is at Y0, Z0 - although I beleive it can be set up to ask for these values upon posting as well. Armed with this information, the post-processor does a 2#!Tload of trigonometry, and everything seems to work.

Don't ask me how to set up MasterCAM to ask for and use the offset values we give it. The local magician (read vendor) took care of that.

The problem with doing it the way we do is that we have to repost every time we set up a part - can't count on fixtures landing exactly where they did last time. Seems that if you let the control do the compensation, you can just punch the new offsets into a table and it does it on the fly with the same gcode every time.