How would I code a surface cut radiused in the y-Z plane around an x axis centerline?

[RogerRetro]

I am new to G-code programming, and simply do hand coding presently. I have designed this little part, for which I have attached a small .PDF of a 3D model. I have been able to code all of the cuts but a couple, for two areas of the model. these are outside 90 degrees of arc curved surfaces running parallel to, and concentrically about a centerline bore.

I have not found any code samples of this type of cut, and could use a jump-start on an approach to the problem. (G2/G3 G18/19 I'm guessing!? - I'm having touble conceptualizing how to handle this.) I hope that between my explanation and the attached illustration, the problem is understandable.

Thanks for any help offered.

Regards,

Roger

[Geof]

I tried looking at your pdf but it did not open correctly. Can you convert the picture to a jpg?

[RogerRetro]

Originally Posted by Geof I tried looking at your pdf but it did not open correctly. Can you convert the picture to a jpg?

Geof, Here it is in .JPG. Thanks for looking.

Roger

[spoiledbrat]

From my understanding, once the G17 mode is in effect, G2 and G3 create circular interpolation in the xy plane. G18 and G19 select the Y-Z and X-Z planes, respectively. Therefore, once your machine is placed into G18, a G2 or G3 move will react appropriately to your needs.

[Kiwi]

When G18 and G19 are used what is the procedure to handle the Tool length compensation?
I tried using G18/19 on my 3axis VMCentre and the tool would move in the relevant perpendicular axis the tool length compensation distance.
ZX Plane = Y axis. YZ Plane = X axis.
The only way I could see how to stop this movement was to enter zero as the tool compensation length.

Sorry to high-jack your thread but I considered this relevant.

[JWK42]

We program a right angle head on our Haas EC-1600. Tool length and tool radius comp do not work. G2 and G3 work with G18 (around 'Y' axis) or G19 (around 'X' axis) but you have to include the tool radius when you program any movements straight or arc. None of the canned cycles work with G18 or G19 mode. We use G10 to set our work Zero. If you have Cad/Cam it should be able to generate the code with out tool L/R comp.
Good luck.

[Geof]

That is an awkward shape to generate without using CAM but here is a way using G18 and circular interpolation.

You will need a 'bullnose or bull' endmill which has a radius on the corner of the cutting edge.

I have done a simple sketch showing the profile of the part. Machine the part so it has a square corner where you want the radiused profile. The bull mill leaves a small radius along the root of the clamping flanges which you want anyway because a sharp square corner here is a terrible stress raiser; it would almost certainly crack at this point with a sharp corner.

The profile is done by starting at the top as shown with the red tool and following the path given by the G18 G02 Y Z and the Y and Z coordinates are the tool position at the bottom of the arc.

This toolpath cutters a circular groove the radius of the cutter so now you go back up to the starting point and move along maybe 0.005" then do the G02 move again. Repeat this for the full length and you have your profile.

You cannot avoid generating a scalloped surface and if you used CAM the same applies. You just control the depth of the scallops by the amount you step along at each pass.

I would write the full code for all the repeat passes by having the G18 G02 move in a subroutine and have the 0.005" stepover an incremental move before each call to the subroutine. All the coordinates have to taken into account both the tool radius and corner radius because tool compensation often is not available for G18 moves.

Like I said above awkward...and tedious.

[RogerRetro]

Thanks for the replies, all...

spoiledbrat,
That helps a little,

Kiwi,
I don't have enough understanding of this stuff to make an intelligent comment.

JWK42,
trying to get my brain around your right angle head just gives me a headache!
and I don't have CAM, so I'm stuck with hand coding at this point.

Geof,
I think I got it... I sort of had this idea, but was getting confused with how to structure it. This gives me something more concrete to work with. I'll get into compensation etc. as I explore the results of my coding...

Again thanks all and Regards,

Roger

[JWK42]

Roger
A right angle head turns a horizontal machine center in to a vertical machine center with a 60" X 40" envelope. We only have a few parts that we do with this configuration. Can't justify a 60" vertical.

[Kiwi]

JWK42
Does a horizontal mill use 'Z' as the vertical or horizontal axis?

[JWK42]

Kiwi
The "Z" is horizontal. In the picture the end mill is along the "Y" axis. I will attach 2 more pics.

[Kiwi]

JWK42
Looks like as standard that the machine spindle axis is considered as Z.

I raised the tool comp issue as I thought Roder would need to consider this while using G18/19.

I now believe my controller parameters are not set correctly as tool length comp is applied on the perpendicular axis(G18 ZX Plane = Y axis. G19 YZ Plane = X axis) when this should only be applied on the Z axis.