Post By Philabuster
What's wrong with this grooving program ???
OK....if someone can take a look at these numbers and see if there is something glaringly wrong here.
Material is 4140 annealed.
Tool: A brand new Iscar GHDR-25.4-3..........designed for grooving and turning. The tool will cut a groove approx. .38 deep.
Insert: Iscar GIPI 3.18-0.20 IC328 (.125 wide)
4 GRV OUT O 1 (W) .19 (FV) 441 (Feed) .001 (DEP) .05 (S-CNR) R.005 (SPT-X) 3.07
(SPT0-Z) .815 (FPT-X) 2.475 (FPT-Z) .815 (Rough) 6
Tool sounds like it's trying to groove rocks. Shakes the whole machine. Wearing and breaking the edge of the insert on the first piece. Actually, it acts like the tool is above center......but that could also be from going too fast.
I've grooved on this machine before with a top notch groove tool, and had no problems whatsoever.....so I'm not sure if my program is too aggressive or perhaps my tool isn't any good.
Also.......with this program, as written, does the tool come in and rough the groove out, leaving stock on the side walls for clean up, or does it come right down to the finish Z dimensions ??? I can't tell when I run program check. I must admit, programming a groove in Mazatrol doesn't make much sense. When it asked for a start point, I want to put the start point at the Z dimension closest to the face of the part and the finish Z to the farthest point from the face.....but the machine wants them both at the same point, which is hard for me to wrap my mind around. When I first started putting the start and finish points the way I felt they should be, the tool wants to make a diagonal cut.....which was quite a surprise. Luckily, I caught that on program check !
Frank, when you select your groove type (0 through 4) it changes which end of the groove you have to give coordinates for.
A "0" pattern groove wants your Z axis point on the spindle side of the groove and then you give it a groove width dimension and I don't believe it leaves finish stock it just plunges I think.
A "1" pattern groove wants your Z axis point for your groove closest to the front of your part opposite of the "0" pattern. This groove uses the finish allowance that you give it.
I would suggest changing it to a "1" pattern, change your Z points to make it correct, and give it some finish stock. Also I'd slow that SFM way down from that 441 to more like 225-250 and feed it .002/rev. This won't be the quickest but you shouldn't have any problems unless your tool height is way off.
Do you have a programming book for the machine? I've been programming them forever and I still have to grab the book sometimes for groove info. They're pretty straight forward once you to speak mazatrol I promise!
To expand further on this,
Originally Posted by Tom3197
When you are selecting your grooving pattern you can push the help soft key and it will bring up a graphic description of how the starting points are called out for each different grooving cycle.
The #2 and #3 are like half grooving cycles. They will only finish one wall and the bottom of your groove. Useful for squaring shoulders in undercuts or whatever you need. I think #2 does the left side and #3 does the right side. Not exactly sure though.
#4 is a partoff routine. It will rough and finish a chamfer and then groove through to part off. Where as the #0 will just take rough cuts and will not take a finish pass.
The Z starting points are sorta tricky at first, and I still refer to the help diagram on the control often.
Disregard my previous post.
Tom and Prawn are correct.
Take the time to play around with the different patterns on a scrap piece of Aluminum if you can as well as use the program check feature.
Which way are your tools running? make sure the spindle direction is right in the cutting cond. page for that tool.
I have a T32-2 control. When I bring up Groove, I'm given I think 4 choices. The first choice looks like a groove. The next choice has angled sides. The next choice after that has a straight side on one side of the groove and an angled side on the other..........then I have a cut off choice. When I hit the button for the choice that looks like a groove, it automatically puts a diamond under the spot which you would fill in the finish information............so basically, as soon as you choose groove, the option of being able to call out a finish pass is eliminated.
I looked at the manual, and it says that I should be able to put finish information in, but as I said before, it is automatically eliminated when I push groove #1.........so this makes no sense.
Also, to answer the question, I run my tools upside down and the spindle running forward.
If you are not sure you can always program all your points
Your first choice is a simple plunging groove. The second choice is a complex grooving cycle that perfoms rough and finish cycles. This option will also allow you to make grooves with one or both tapered walls, grooves cut in at an angle and gives the ability to form chamfers and radii on the edges of the groove.
Originally Posted by rockfish
So... Use the second option. Specify finish stock allowance at about .005 or so. Specify same tool for rough and finish pasess. Specify starting corner chamer or radius size if a nice burr free edge is desired. Start and finish point X values will be the same. The start and finish point Z values will be .625 in this type.
Maybe slow that speed to 350 ft/min for the rough pass and give it about .004 feed or so. Set the finish pass at about 450 ft/min and 5 or 6 finish. You should have great results.
At the speed/feed combination you listed, the chip could have been getting trapped in the groove causing galling and loading on the tool. It appears you had a .05 peck depth which is a good thing. Keep that in there.
It would seem to me that the tool would have to be noticeably off center (high) to cause a problem at the diameter you are cutting. Make a manual face cut and watch very closely as it comes to center. You could definitely see it.
And yeah... I would just for the heck of it slow the spindle over ride down enough to make positively sure it is running forward.
Hope that helps.
Last edited by SDI-Gary; 05-12-2012 at 10:10 AM.
Reason: typso... tpyos... typos dang it.
I have to say Gary nailed it except spt-x should be 3.07 and FTP-x should be 2.475.
I never use GRV type 0. You have to use the Z-dimension of the groove closest to the chuck (which is opposite most of the other GRV types), and GRV type 0 does not let you put a chamfer on the top corner of the groove.
Use GRV type 1 for most any groove you will do. It chamfers both sides of the groove on top, and will radius (or chamfer) bothe sides of the groove at the bottom. The program Z dimension is towards the "Z-zero", or faced-off end of the part.
GRV type 1 should give you a FINISH allowance, and thus a rough and finish tool callout. Use the same tool # for both R & F.
The finish allowance in the GRV unit determines how much the R groove tool will leave on the sides and the bottom of the groove. The finish allowance you specify in the very first line of the program does not apply to grooving.
Slow you SFM way down, all the way down to 100 SFM, if you have to. Bump the feed up to .002 or .003.
Good luck Frank!
I agree with everything here for normal OD or Face grooves.
Originally Posted by cnctoolcat
However, regarding GRV type 0, there are circumstances where it is very handy to use. The limitations the Catman pointed out are no chamfer on top of groove or controlled radii at groove bottom--you get the radius on the insert. This groove process is designed for a one shot tool motion--BUT that does not mean it has to be only used as a finish tool or finish groove operation as implied in the program.
The main use of GRV 0 is an undercutting groove motion, ie, this can groove the intersection OD and face corner at 45° for a grind relief. If you use two GRV 0 processes with different start points, but the same end points, you can create a groove with a 45° on one side and say a 60° angle on the other side. This is the ONLY process in Mazatrol that will allow motion in +/- in both X and Z axes in one process besides the manual G-code MNP process.
The other advantage is roughing out a groove with #0 and finish with #1 will cut the roughing cycle time of the groove in half (same tool in turret or using two different tools). No big deal for one-off parts, but it helps when you are shaving cycle time on a production job. Reason being is GRV 0 just goes plunge, plunge, plunge, done. GRV #1 plunges center, then roughs out right side, then roughs out chamfer, then repeats same on left side. Really no reason to rough out a .010" chamfer at the top of the groove, but that is how the macro is designed.