We just got our new TL2 and we are using the IPS programing to start with, we cant seem to figure out how to change the finish pass dimensions? Or if we can do that at all. On OD turn it isnt an issue but when we face a part it takes it down with beautiful roughing passes, and on the finish pass it takes basically a "spring" pass. Which makes the finish look like ass. I know the easiest way to take care of this is to just start fresh with our own G Code but I still think there should be a way to change this in the IPS programing. Thanks
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
TL2 IPS finish pass
- Thread starter Butch1
- Start date
- Replies 13
- Views 3,326
CBlair
Diamond
- Joined
- Sep 23, 2002
- Location
- Lawrenceville GA USA
I believe that value is set by a parameter setting, your rep should be able to help you change that if you want to.
Charles
Charles
Justice25
Plastic
- Joined
- Jul 30, 2009
- Location
- Lake City, TN
on ours, if you have .025 to face and your depth of cut ends up with the last pass taking .025 then you will have a finish pass which takes nothing. for instance if you are taking .025 off the face and have your depth of cut set at .035 it should only take 1 pass, but if it is set at .025 it will take 2, one being at the same z dimmension as the last, and if it is set at .02 it will take .02 the first pass and .005 the last pass, does this make sense?
Yeah that makes sense, but we have tried different depths with the same outcome. But it only happens on facing. We have taken .100 with .025 depth of cut and it will take 4 cuts at .025 and a last cut at the same place as the prior. Which basically "shaves" the face and the finish goes to hell.
Hdpg
Stainless
- Joined
- Feb 19, 2009
- Location
- Vancouver, B.C. Canada
Does IPS use the G72/G70 facing canned cycles? G72 does the same thing, a final spring pass at the same position asa the last cut. This is where G70 comes in because you can have a W value in the G72 which leaves a finish allowance that is then removed by the final G70 pass.
It is using G72. We read that G70 would be what we need to use but cant seem to find out how to change it in the IPS. We like using the IPS for most of the parts we make because they are usually either one off's or a low production # like 10-20. And with those type of parts I can program with the IPS at the machine and figure out workholding and be making chips before we can write a program in CAD/CAM.
Hdpg
Stainless
- Joined
- Feb 19, 2009
- Location
- Vancouver, B.C. Canada
The G70 command just uses the same P Q blocks as the G72 and goes directly after the Q block; you should be able to edit it in by hand.
The real advantage of using G70 is that in the P Q block you can specify slower feed rates for the finishing cut which are ignored by the G72. You can also increase the spindle speed or CSS surface speed setting and change to a finishing tool before doing the final pass.
The real advantage of using G70 is that in the P Q block you can specify slower feed rates for the finishing cut which are ignored by the G72. You can also increase the spindle speed or CSS surface speed setting and change to a finishing tool before doing the final pass.
Justice25
Plastic
- Joined
- Jul 30, 2009
- Location
- Lake City, TN
try taking .100 with a depth of cut of .026 and see if it takes 3 cuts of .026 and a finish cut of .022.
Hdpg
Stainless
- Joined
- Feb 19, 2009
- Location
- Vancouver, B.C. Canada
The G72 canned cycle will do this but sometimes it does not help with the finish because it will do a final pass at the same coordinate, and this, almost non-cutting pass, can leave a worse finish than that from the 0.022" cut.
Born2L8
Hot Rolled
- Joined
- Oct 10, 2006
- Location
- Richlands, VA
Hdgp, you get the prize. But why in the world is there not a finishing cycle in the IPS. That sucks!
Charlie
Charlie
Hdpg
Stainless
- Joined
- Feb 19, 2009
- Location
- Vancouver, B.C. Canada
Don't ask me, I don't own Haas Automation.
Maybe Haas Apps is monitoring this thread and can make a comment. I never bothered figuring out the IPS because I could already hand code so fast on a lathe before I got a TL2. I just have what I call template programs for all the common operations and I just edit coordinates for different jobs.
athack
Stainless
- Joined
- Nov 2, 2009
- Location
- Michigan USA
The way around this issue I use is to add a finish cut. Using IPS leave the part longer then needed by the amount the insert needs to break a chip to cut a good finish. Then IPS in one more cut, says you need .025 to acheive the finish and use doc of .100. The machine will cut it in one pass. Thirty seconds of programing and 10 seconds for an extra cut.
