Right Angle Head Programming

Can someone please tell me how you would program (G-code) a right angle head attachment on a 3-axes verticle machining center ?. How would you compensate for the tool length & tool diam ?.

thanks

Ed

What kind of RAH? Are you using milling cutters on this or endmill/drills? Either way it does not make much difference what kind of tooling you are using.

You should always go from the centerline of the cutting tool. Any adjustments that need to be made for tool diameter can be done in tool radius offset page.

I have attached a sketch using disk mills.

Stevo

I would do it the hard way (mix of manual and automatic programming) and step through the moves very carefully :D

You will not be able to compensate for tool radius too handily in planes out of standard position so don't waste time trying to make G41/G42 work, just program directly to tool centerline.

As for tool length compensation, you will need to use the Z length compensation to define the center plane of the tool's horizontal axis, as in the distance from the spindle gage line.

If you are doing this in cam, you could reckon the tool to be similar to a slitting saw on an arbor. The radius of the saw would be equivalent to the distance of the tool tip from the machine spindle centerline. The mid plane of the saw would be equivalent to the right angle spindle's centerline, and the saw thickness would be equivalent to the diameter of the cutter.

This sort of visualization may help you to determine if the approach of the tool is being done in a crash free way.

Suppose you have the tool set in such an attitude that you can drill holes with Y movements of the table. Touch the end of the tool off the relevant part face and set that position as your Y workshift. Set the X workshift to some datum on the part, and set the Z workshift on a top feature of the part, remembering to add the thickness of the tool radius to this position, because you want to program to the center of the tool. This workshift is only relevant to this tool and absolutely should not be used for any other tool!

This should make the position of the part face to be Y0 when programming. For the sake of clarity, Y+ absolute positions should be in the clear, and Y- absolute positions will be cutting (depending on the orientation of the part, of course) so that code troubleshooting is easier to do.

Gcode cycles for drilling ops are likely not going to work in this plane, you'd be looking at coding drill cycles out long hand.

I'd try to stick with profile type movements if I was using cam to make positional movements or actual profile cuts. Using automatic comp (not machine comp), you can then make use of the lead in/lead out amounts to create your depth of cut. Make sure that those movements are perpendicular to the part face in the relevant plane.

If you need to actually mill using XZ or YZ simultaneous movements, that would be considerably more difficult to do in cam. In such an case, I would probably draw the pocketing toolpath out as a backplot (in XY), then rotate it into the part orientation as the part sits on the mill. I would use simple "follow 3d chain" type machining strategies to generate code that follows that geometry. Again, carefully add lead in and lead out movements where needed, and make sure that no automatic Z retractions get posted. If you see that happening, then break the geometry chain as needed, add the lead in and lead out to every dead end start/end point. In simulation, if you use a slitting saw type tool description, this should help alert you to crashes due to unforeseen Z retractions. I don't say that the simulation will be much good for anything other than watching for entry gouges, the retraction gouge is equally dangerous, but won't show up as a gouge warning in 3 axis cam.

Make sure the tool comes clear of the work before it rises to clearance!

Create the program as your part is on XY Plane.
Rotate Y plane 90 deg.
With a FAGOR controller use G49 B90.
Fanuc G68 'Coordinate System Rotation'

Thanks for info. I will give that a try.

Hu.... what are you talking about??

Quote:

---

You will not be able to compensate for tool radius too handily in planes out of standard position so don't waste time trying to make G41/G42 work, just program directly to tool centerline.

---

Should be able to use G18/19 depending on head orientation... I do. Cutter comp works fine.

Quote:

---

Gcode cycles for drilling ops are likely not going to work in this plane,

---

This is true. However, some MTB's will have it written in to change drilling direction by use of 2D/3D rotate (G68) or by plane select. This allows for canned cycles.

However, many controls are capable of changing drilling axis by parameter. (PITA... especially if you forget to change it back!)

Hi Psychomill. Im trying to comp the dia of a tool using a 90 degree head on a HAAS VF-6 and Im getting a comp alarm. Can you show me an example of where the G18/G19 should be used in the Code. Does it replace the G40? Thanks

Hi,
I have a 45 deg head for drilling and endmill. I have programmed it to the center of the tool. The NC code is following YZ plane and looks ok to me. But on the machine the hole looks out of round as if the endmill has not cleared the Drilled faces.
I suspect the tool offset to be incorrect. What’s the best way to take tool offsets on a 45 deg head when you want to machine from the center of tool?