variable angle drilling head

[kendo]

I got some parts coming at me in the next month that get drilled at an angle
of about 81.5
theres a drilling head thats not here yet which will be used for this and Im trying to get a jump on things, as I've never done anything like this before
I'm not sure whats going to be the best way of setting up my offsets with this drill sticking out to the side of the spindle centerline
I drew some cad (below) showing the initial X,Z location in relation to the part,
and the endpoint of the drill path in relation to the initial location

so telling it to drill like this:
G1 G91 X-.5044 Z-.0747 F20.
G0 X.5044 Z.0747
should be no problem,

But how would you get the drill point to the initial location?
I know the geometry I dimensioned that location from is probably not the best,
but thats my question, how would you pros tackle this?
I do have the renishaw probe and tool setter at my disposal.

[bshields]

Try working from the pivot point of the angle head to the end of the drill. If you know that, along with the angle, it's all you need.

Everything else is done with basic trig - so get the length to the pivot known and you are home free...with the tool.

Actual location of the point in question is also, just basic trig. You can work it out from your CAD drawing and known origin location without too much trouble.

REMEMBER however, that very few controls will run a CANNED cycle at a funky angle, so you have to G1 XYZ Feed your way in and G1 XYZ feed-high on your way out. Do NOT use G0 to retract unless you have a lot of drills.

If you have a control that will allow you to set a local, rotated coordinate system, then you can use canned cycles...but then if you had one of those controls, you probably wouldn't be asking this question.

[Matt@RFR]

I've never done anything like that so I'm no help with your main question, but I do have a suggestion: Don't rapid out of the hole. Haas uses dog-leg rapids and because you're at that angle, it will probably hit the hole on the way out. Instead, G1 out of the hole at a fast feedrate and it'll go in a straight line.

[kendo]

Thanks guys, I hadn't thought about the rapid issue, even though I've watched this machine rapid hundreds of times and one axis always reaches its programmed position first.
I have ten times more experience on the Tree mill, and its axes arrive simultaneously.

As for trign' from the pivot position, that oughtta be a piece of cake too, once I look up those triangle equations again. And as long as I know the distance from the center of pivot to the tool tip.
Thanks again y'all.

[Kiwi]

Can you rotate the XY plane 81.5deg (maybe 8.5deg) with your controller. With a Fagor I would use G49 B81.5. Now the XY plane is perpendicular to the hole and can be machined the same as if perpendicular to the table.

[kendo]

that I'd like to know, I don't think the Haas will let me though since its not a 5ax machine

so far it looks like the G68 rotation is just for rotating a programmed feature about a point on a given plane, G17 being the X,Y plane

[Kiwi]

Originally Posted by kendo that I'd like to know, I don't think the Haas will let me though since its not a 5ax machine.........

The machine doesn't need to be 5 axis, my machine is a 3 axis vertical mill with a Fagor 8055M controller. I don't know whether Haas or Fanuc has this feature.

[kendo]

The Haas manual says:

G-184:
This G code is used to perform rigid tapping for non-vertical holes. It may be used with a right-angle head to perform rigid tapping in the X or Y axis on a three-axis mill, or to perform rigid tapping along an arbitrary angle with a fiveaxis mill.

I think thats a "No"

[Kiwi]

kendo
From what I read, I believe that you can activate G18 (XZ Plane) and then G68X0Y0R8.43 (X & Y being Centre Point and R = Angle of rotation). G69 to cancel
If you try, watch out for unexpected moves for tool length compensation. This may not apply to your machine.

[kendo]

I'd like to know what you're reading,
the manual Im reading (Mill Operator's Manual Jan. 2007 96-8000 revP)
has 2 pages about G68, and all it talks about is rotating coordinates about a specified center on a given plane, nowhere does it say you can rotate the plane itself.

then its says in the section about G184 that the ability to execute canned cycles on a plane thats rotated to an arbitrary angle is limited to 5ax machines

this is something I've never ventured into, so maybe I'm not thinking about it correctly

[Excelmachine]

Why not just do the drilling as a secondary op? Saves having to buy an expensive drill head.

[Kiwi]

Originally Posted by kendo I'd like to know what you're reading,................

I'm getting my information from 'CNC Programing Handbook' by Peter Smid.
This book calls G68 'Coordinate Rotation' where the Fagor Manual calls G49 'Incline Plane Definition'.
From what I read these are similiar. With a Fanuc, G68 appears to rotate the coordinates on ONE of the 3 planes.
With a Fagor, G49 feature can rotate the plane around the X axis first, then Y axis, then Z axis.

If G68 works like I think, when you run:

G18
G68X0Y0R81.5

All movements (jogging or by code) will be relative to the 81.5deg setting until canceled.

Whether you see it as rotating the coords or rotating the plane, I see this has the same outcome but sometimes I'm wrong. Best test will be to try it.