Lathe groove

[JPensack Acker Drill]

Is there a quick way to set my approach to feed rate and at a 45 deg angle for grooving? On an internal groove I am using a reference point of z1.0 then I want it to rapid in to about .1 away on x and z. Then feed it at lets say .03 then feed at .003 then retract the same way. I do alot of grooves up against shoulders and it defaults to rapiding in to the z depth and then feeding straight in on x. I've used toolpath editor but it becomes a pain when I have alot to do.

[Philcott]

In X2 I don't believe there is a quick way to do what you want in the roughing part of the groove. You can make limited settings for lead in for both first and second pass but there is nothing for lead out.

[wham58]

What is the width of the groove you are cutting and the width of the tool?

There are different tricks to approach a rough groove versus a finish groove.

It sounds like you want to start your 1st finish wall on the bottom of the part and feed into the wall at a 45 deg angle at a feed rate of .003 from .03 away?

Is that correct?

There are more options to do what you want with a finish pass than with a rough pass as the rough pass does not offer lead in.

[JPensack Acker Drill]

I am just doing the groove in one shot with the appropriate size tool. With a rough and finish groove its no problem since their is the lead in and out. Alot of our grooves are 1/16th and 1/8th for o rings. So the grooves I'm speaking of are just a one shot groove. The approach would be approximately .1 in x and z, with a feed of .03 then when I get to like .01 way switch to .003. MC likes to tell me in verify that I have a colision but its just the groover rapiding to its position and then feed.

[gcode]

Try this..

draw a line representing the .003 IPR segment

of your groove.

Chain it and use a finish toolpath.

Use a tangent lead in of the appropriate distance

and set your lead-in feedrate at .030

and a retract feedrate with a negative value

big enough to get you back out of the cut

You can crank up the retract feedrate or switch to rapid.

[wham58]

I tried playing around with this a little.

2 point works good if there is no chamfer or radius involved.

To get a good 2 point tool path with the cutter the same size as the groove, turn off the rough toolpath. In the finish tab change the finish step over to 0. I turned the wall backoff off also.

With stock setup the tool will preposition in front of the stock.

With the finish toolpath you get lead in. It doesn't give you all the control you were looking for but it does feed into the bottom a little more gently than a rapid. If you need a chamfer or a radius create it afterwards with a finish TP.

to get the finish TP to work correctly you will need to go into the plunge paramters and change the tool width compensation to use tool width. This will allow you to cut on the back side of the insert for the chamfer or radius.

Hope this helps.