Lathe groove

[K2csq7]

X5 (no mu1)

Lathe groove, using chain, using stock for outer boundary... On the roughing tab, whatever I put in for "Stock Clearance" is how much the tool will "back up" before plunging. I am using depth cuts and tool inspection, it doesn't start happening until the 2nd or 3rd depth cut. Anyone know how I can get rid of the backing up?? If I set the "Stock Clearance" to zero I get the "Tool collision with stock" error (which makes sense).

 

TIA

 

 

 

[DODGERFAN]

use stock for outer boundry and set stock amount at .000 on rough perameters page use stock clearence, i use .10 for all grooving

[Tony35]

did you try to change the stepover amount?

just taking a stab here

[K2csq7]

Thanks guys.

Dodgerfan, my settings are identical to yours... I did also try unchecking the "use stock for outer boundary" and using the "stock amount" instead, same thing.

Tony, the width of the opening is only .220 and I am using a .157 wide tool... Just 2 steps (side to side).

I just tried adjusting it down to 10% of the tool and it didn't like that at all. Still have the backing up issue.

 

The same thing happenned to me the other day making a .125 wide ID groove with a .125 wide insert. Using depth cuts, after the 2nd or 3rd depth cut it would rapid into position then back up then enter the cut.

 

I am using the tool inspection feature set to go to my "user defined" position after every plunge, I shut it off to see if it made a difference but it did not.

[K2csq7]

I created a dummy file with the problem in it.

 

The first 2 plunges are fine, but watch as the 3rd & 4th plunges start (backplot)... The tool rapids to position then backs up then goes in...

[Tony35]

Keith

i dont see any toolpaths in the Z2G

 

is your lead in/out causing it to pull back (wrong angle, length of lead)

[K2csq7]

Not using any lead in/out finish tab is unchecked... only using the roughing tab.

See if the file below works better...

[DODGERFAN]

HOW DID THAT WORK KEITH?

[K2csq7]

Dodgerfan, thanks for the email. Changing the "retract to stock clearance" in the depth cuts window from absolute to incremental and unchecking tool inspection eliminated the "backing up", but I need to have tool inspection on and with it on the thing still backs up...

[DODGERFAN]

Dodgerfan, thanks for the email. Changing the "retract to stock clearance" in the depth cuts window from absolute to incremental and unchecking tool inspection eliminated the "backing up", but I need to have tool inspection on and with it on the thing still backs up...

Well that sux

[K2csq7]

:lol:

[DODGERFAN]

ok, uncheck depth of cuts and check peck groove, that fixed it here

[K2csq7]

Yes that works, but I need to be able to have the tool retract for inspection after every plunge/cut. I really don't think the insert will go 1" deep in Waspaloy Each cut gets a consecutive "N" number (1.2.3.4....) with safe start codes.

 

Gonna use it for now and just make the operator aware of the funny moves.

[DODGERFAN]

Yes that works, but I need to be able to have the tool retract for inspection after every plunge/cut. I really don't think the insert will go 1" deep in Waspaloy Each cut gets a consecutive "N" number (1.2.3.4....) with safe start codes.

 

Gonna use it for now and just make the operator aware of the funny moves.

change your peck depths to around .075 and rock on!

[K2csq7]

Sent this one into QC, it has now been logged as "CNC00097228".

 

Workaround is shut off "use stock for outer boundary", set "stock clearance" to zero, and use the "stock amount" for whatever value you need for clearance...

[Dan@home]

Change your Cut Direction to Positive instead of Bi-Directional. I think it is because the groove tool is the same width as your groove, and it is trying to move bi-directional and can't because there is no room.

[K2csq7]

Dan, changing the cut direction definitly helps, thanks!

But the other stock settings need to be played with a bit for grooves that are wider than the tool.

Definitely a bug in there somewhere....

[NOTW Programmer]

Dan, changing the cut direction definitly helps, thanks!

But the other stock settings need to be played with a bit for grooves that are wider than the tool.

Definitely a bug in there somewhere....

Just had an instance today where the tool would plunge to the center of the part then peck up to the geometry in the increments defined in the peck groove page. Chaging the retract moves from absolute to incremental fixed it, if you want to use absolute you have to include the parts OD I guess.