taper in grooves

[newmachinist]

Hi I've been a machinists for 6 months now and have been running an old fanuc OT lathe. I have to make parts with .002" tolerances, which is difficult. The biggest problem I'm having is trying to make inside grooves without taper. I am competent enough to write a taper line in when the tool goes to make the finish pass, but it only effects the ends of the groove. Just wondering if anyone knows how to write a taper line that will also get the taper out of the middle of the groove. I hope I'm making sense to anyone lol.

[rookiepro]

What material are u working? What are your feeds and speeds? What does your surface finish call for? What is your tolerance on angles?

[newmachinist]

I work with ductile iron. Depending on the amount of chatter I run the speed 500 - 600, and feed rate between .005 and .010. I don't know about the angle. It isn't listed in the blueprint or program, but the groove does have a .015 radius if that's what your talking about. Surface finish <64.

[angelw]

Originally Posted by newmachinist

I work with ductile iron. Depending on the amount of chatter I run the speed 500 - 600, and feed rate between .005 and .010. I don't know about the angle. It isn't listed in the blueprint or program, but the groove does have a .015 radius if that's what your talking about. Surface finish <64.

Post a sketch of the groove you're machining, and specifications of the Internal Grooving tool being used, ie. bar diameter, width of insert, and corner radius. More information is needed to give you a viable suggestion.

1. You make mention of the groove requiring a 0.015 radius, is this a corner radius between the bottom surface and the sides of the groove?

2. Is the 0.005 and 0.010 feed, the feed in X for the sides? If so, and if using 0.010, this is a fairly hefty feed. If the 0.015 radius is as in point 1, the corner radius of the insert can't be larger than 0.015. Accordingly, you will not achieve <64 surface finish on the sides of the groove using the combination of a 0.015 corner radius insert and a feed rate of 0.010.

Regards,

Bill

[newmachinist]

For this particular part I use a 1.5" GB with a .125" carbide insert (MT cp500). I'm making a 2.503" deep groove 1.03" wide in a bore that's 2.26". the radius is .015 on the bottom of the sides because of the shape of the insert I imagine. try to bear with me, I'm still learning. The program plunges to 2.5", puts a chamfer on each side then sweeps the remaining dept. On top of that I have to add a .002 taper line in the sweep.

[angelw]

Originally Posted by newmachinist

For this particular part I use a 1.5" GB with a .125" carbide insert (MT cp500). I'm making a 2.503" deep groove 1.03" wide in a bore that's 2.26". the radius is .015 on the bottom of the sides because of the shape of the insert I imagine. try to bear with me, I'm still learning. The program plunges to 2.5", puts a chamber on each side then sweeps the remaining dept. On top of that I have to add a .002 taper line in the sweep.

If you're referring to a taper in the 2.503" diameter of the groove from one end to the other, you can do as follows for the example given

1. Z start coordinate = Z-0.500
2. Z finish coordinate = Z-1.405 (this includes the width of the insert - 0.125")
3. Taper in diameter = 0.005", smaller at the Z-1.405 end of the groove

The program block, with the tool at X2.503 Z-0.500 would be:
G01 X2.508 Z-1.405

With grooves that have a specified tolerance for the position of both sides of the groove, 2 Tool Offsets can be used, 1 applied to each side of the insert. Using this method allows the position for each side of the groove to be regulated via the Z offset for the associated side of the insert.

Regards,

Bill

[newmachinist]

yeah your exactly right Bill, and it does eliminate taper on both ends of the groove, but for some reason there is still a .001 "bulge" in the center of the groove even if both sides are the same measurement. Apparently my machine cant cut a straight line. For example: If one side reads 2.503" and the other 2.501" I'll add a taper line just like you said and get both sides to measure 2.503", but the center will read 2.504".

[angelw]

Originally Posted by newmachinist

yeah your exactly right Bill, and it does eliminate taper on both ends of the groove, but for some reason there is still a .001 "bulge" in the center of the groove even if both sides are the same measurement. Apparently my machine cant cut a straight line. For example: If one side reads 2.503" and the other 2.501" I'll add a taper line just like you said and get both sides to measure 2.503", but the center will read 2.504".

You can get errors such as you describe through wear in the slides, but its normally noticeable over longer lengths; not over a short length such as 0.905".

Often you see a slight reduction in diameter where the tool initially feeds down to depth due to push away between the grooving bar and workpiece, caused by the width of the grooving insert, but that does not explain why the finish end of the groove would be smaller than the centre.

You could program the finish pass of the groove as follows as a work around.
Starting at X2.503 Z-0.500

G01 X2.5045 Z-0.9525 this will compensate for the 0.001" hollow in the centre
G01 X2.508 Z-1.405

Have you ever checked the Headstock of the machine for parallel alignment with the Z axis?

Regards,

Bill

[newmachinist]

im positive its because of that old ass machine. Maintenance has looked at it, but there doesnt seem to be anything they can do. I understand what your saying and will definitely try it out. Thanks All!

[littlejohn]

i would deffinately check the ways of the machine, even a small nick or bur along the gibs or shoe can cause this. it might be bar spring in which case, take a lighter finish cut. if there is chatter with the lighter cut, slow down the rpm