Thread: Face Groove Problem

We are having trouble profiling a large face groove. The groove is 3.189" wide and 1.289" deep with face radii of .500" and bottom of groove corner radii of .552". We are using the Face Groove command and are getting incorrect radii (larger) and have to increase the offsets alot to get the correct diameters.
Tooling is a round .250" radius insert, pretty sure we have the tool entered correctly.
Anyone have any suggestions.
Control is a T3(CAM) on a Slant Turn 40N.
Thanks,
Jeff

I've had similar problems getting our 640T to give me the shapes and tolerance needed using the "Groove-Face" options.

Right now I'm fighting a series of grooves on the flat face of a forming die that look like (and almost measure the same as) a lightbulb thread. I'm getting the screwiest stuff you've ever seen, and when it finally renders on the 'check shape' display, it'll lock up on the 'toolpath' display and give me an incorrect data error.

Tried going to the "Bar" type and using the radius toolpaths to contour rather than groove? That's my next ploy.

Old fashioned tool pressure maybe? What type of
material, sometimes it's better to make a lot
of quick shallow passes, than slow deep ones.

I know what are you talking about, I have the same problem. It's is kind trick to program. I program from center of the radius. For example, the tool radius is .05 and the part is .1RAD the program will be .15Rad. Since you use mazatrol, It must program in MNP.

The downside program like is you must use the same tool radius everytime.

Sometimes that is a result of the tool description in tool data 2. If you program too large of a radius the machine will refuse to do it. Sometimes you have to lie to the machine. I've run into this problem with face grooving and cutoffs. EX: I tried putting a .125 radius champher on a cutoff. The machine threw up an alarm. What I ended up doing was saying my cutoff was a .250 width, then I moved the groove over .125 to compensate. Judging from the size of your tool and the size of the radius you're attempting, that may just be the problem. Then the machine would do it. Otherwise, MNP is your only hope.

Oh, my cutoff tool was .125 wide to begin with. Sorry.

Jeff,
Cut my grooves with a full-nose radius tool, (.062w, .031rad) using the "Taper" command in "Bar" and just invoking a beginning and ending radius....failed miserably.

Good looking grooves, to be sure, but not at all to spec. On top of that, the top of the grooves is BELOW the Z-zero even though they're programmed to crest at zero. The good news is the program works, and by tuning it I'm sure I can bring it into spec.

Interesting exercise, but I don't think I should have to play these games with it.

Next iteration? I'll use the inside and outside radius contour commands. (only reason I haven't yet is the drawing has got stupid dimensions, that I've yet to calculate)

1: Describe the tool as a regular face groover .5"
wide
2: set the "r" value @ "0" (zero)on your tool data
page

3: program your corner radius on top and fillets @
the bottom of the groove as "print "R" minus
radius on tool.
this will eliminate the thinking/calculating process of the controller and do a "point to point" move

been there done that, many times

Lie lie lie mazatoal is the liers favorite. Mazak calls it manulipitating the data I call it lieing.Tough thing about mazatrol is learning how the machine wants to do it and working with that.Sometime the easiest thing to do is lay every part of the process in question out on cad and write a manual process to do the job not using tool radius comp. If the tool is used in another process on the same program set it up as a diffrent tool in the same pocket example (tool 3 is a face grooving tool with a .5r. tool3a is a bar face tool with a .000 r. and do it with tool 3a, tool 3b can be a turning tool the possiblities are almost endless) I hope this is of some help Good luck Calvinator

Lie lie lie mazatoal is the liers favorite.

9IT IS "MAZATROL" NOT "MAZATOAL"

>>>>Back in the day, when a machinist got a cnc to do what the basic controller wouldn't allow it to, the shop Foreman gave the machinist a big attaboy and called it "INGENUITY" not lying. Times have changed I guess, I do miss the good ole days!!

A big attaboy to all of you out there that use INGENUITY to get the job done instead of lying to the machine

SteelCutter

DOGGYDOOO, HERE I'M CORRECTING calvinator'R SPELLING AND I SCREW UP MYSELF!!

STEELCUTTER

sorry bout the caps in my previous post

SteelCutter

Check the radial position of the turret. it is a good idea to do this once per month. If the turret is out, it will affect some of the previous programmes when corrected.

Had good results using Mazatol face grooving, machining from the smallest diameter 3mm face cut depth .08 feed then facing out to the large diameter. Had good results using 6mm width x .1 rad insert.

Use roughing and finish turning tools