What's new
What's new

Programming Help

Mike_H

Plastic
Joined
Apr 11, 2003
Location
Butler, PA
I need a little help- I am just learning basic programming. I can do quite well with my HAAS tl-1, but when it comes to writing my own programs I still get stuck easily.

I currently need to machine this simple feature on the OD of a 1-1/4" round bar - a concave groove, 1/2" wide and 3/16" deep, or the diameter reduced to 7/8". The shape is rounded with a 1/4" radius specified. How would you write this program? I was going to round off a 1/8" grooving tool to make the cut. In the same area- I once tried to cut the same type of groove for a tube bending die. I'm sure this is obvious to many of you- but after hours of frustration- show me the light! :confused:

Many Thanks!!

-Mike
 
I would probably use an Iscar cutgrip style tool, and purchase a full radius insert for it. By full radius, I mean a completely round nose insert, with no flat spot, in other words, not a bullnose tool. The advantage of using a commercial insert is that it will have some chipforming capability (if you buy the correct one), and the tool radius will be an assumed truly formed curve. Probably a 2 or 2.5mm radius tool would serve the purpose.

Make a starting plunge right in the center of the groove position. Go within a few thousandths of full depth.

Then create a left side toolpath and a right side toolpath. The toolpath would be bell-shaped, taking successive increasing radial cuts, starting at the OD near the center of the groove and moving down towards the plunged groove that was made initially. Work your way over til your final cut contours along the groove curve. Repeat on the other half of the curve.

If you like, you could take a really skimpy finish cut from one side to the other, but on cnc, this is generally not necessary, because it is not difficult to stop exactly at the bottom of the groove, retract and come down again.

You can offset the geometry to allow for your tool radius, if you are calculating all this longhand. Take care that your initial tool offsets would need to be corrected for reference at the center of the tool radius, rather than at its normal tangential touch off points.
 
Yup, as Hu said. The Iscar CutGrips are really nice.
To write the code though, use the G71 roughing cycle, put in cut-comp left, no W. Move to .1 or so above your X start point, maybe .1 in front of the Z and just write the whole thing. If you only want the groove, then the code will be 4 lines:
G00 G42 (start point)
G71 D.. P10 Q50 U.. F..
N10 G01 X.. Z.. <- start of rad, Must have X and Z
N20 G02 X.. Z.. <-end of rad.

done.

Now I'm not sure on the TL with the tool being in the front you may want G41, but the idea is the same.
 
Here is a quick example what I was talking about.
I've made the radius start at Z-.5, so the groove C/L is at Z-.75.


G00 G97 T101 S600 M03
G00 G42 X1.75 Z-0.5
G96 S300 M08
G71 D.05 P10 Q50 U.008 W0 F.008
N10 G01 X1.25 Z-0.5
G02 X1.25 Z-1. R0.2604
N50 G01 X1.75 Z-1.
G00 G40 X2.5 Z.1

Again, this assumes the SL series lathes, where the tools are in the back < hence the G42 >, and that the 1.25 dia is all done, you're only doing the radius.

To go back and finish with the same tool, just add the following at the end:

G00 G42 X1.75 Z-0.5
G96 S300 M08
G70 P10 Q50 F.005 <- finish cycle.


Lastly, this is using a full radius insert, with tooltip defined as direction 8, proper tip radius entered.
 
The part is about 8" long, and the groove is near the middle. I'll try the program tomorrow. I will probably make my own tool for this one, since I only have 10 parts to make. I've read some other threads on Iscar and am going to give them a try. I just finished a job where I was parting 2-1/4" free maching bar and was using Hertel inserts, trashed 1 blade and 8 inserts for just 180 parts. I'm sure I was doing something wrong, but never did completely figure it out. Thanks!!
 
Mike

I did draw that part up quickly, and a VNMG will do the groove no problem. It has 47deg. back angle, and you'll be fine.
8 inserts for 180 parts? Not bad if it's Inco, but for steel? That ain't right! Speed/Feed?
 








 
Back
Top