Correct chamfer/radius on TL lathe with IPS

Hi,

On my TL-1, when I try to do a fillet or radius with the intuitive programming the size is too big. This applies to both inside or outside cuts. When I first got my TL-1 about two years ago I somehow figured out how to trick the control into giving me the correct radius of a fillet or size of chamfer. I took about 1.5 years off from the lathe and now I can't figure out how to do it. What is the trick to this? I input the correct tool nose radius on the IPS screen. I also have the radius listed on my tool offsets page. If I use VQC, everything works fine. But, VQC won't do just a chamfer or radius, they are part of some "bigger" operation.

Thanks,
Eric

I wish I could help you. My TL-1 cuts radius and champhers fine from the ips. I just input tnr in the tool offsets page and fill in the blanks in ips and that's it. Let us know if you figger out the problem.

send your code to MDI and see what the numbers look like, they should match up with what you have entered. If not perhaps there is some kind of scaling factor someplace in the parameters.

Charles

After reading your post I IPSed a radius on my TL-1 and it cut it perfectly. Entered rdius and tool nose radius and thats it.

Maybe one of your settings is set to something other than zero. Happened to me once all parts where coming out .110 short. Can't remember which setting it was but just went through and checked till I found something od.

Let us know what you find.

I dug through all my settings and parameters and couldn't find any obvious culprit. I did change Setting 85 (max corner rounding) to a little lower number, but this shouldn't affect fillets.

Anyhow, maybe my memory from 1.5 years ago is faulty. I tried a few fillets and they were spot on. I also tried a few chamfers and they are still oversized, though. I did figure out how I "tricked" the system before into giving me correct chamfers. In the operators manual, there are two pages with "Tool Radius and Angle Chart" (p 73 and 75 in the June 2008 online manual), one for 1/32" tnr and 1/64" tnr. These charts are used with other pages in the manual in showing how to do tool nose radius calculations on chamfers.

When I tried doing my first sample chamfer I wanted a .025" chamfer. As close as I could estimate it was measuring more like .040". The tool I was using had a .0312" radius. I then mostly remembered what I figured out in early 2008. I used the table in the manual and took the number from the Zc longitudinal column for a 45deg angle (.0183" for 1/32" tnr and .0092 for 1/64" tnr) and subtracted it from my desired chamfer. So, instead of putting .025" in IPS for my chamfer size, I put .0067". That resulted in my correct .025" chamfer on the part. I tried this with other tool nose radius tools (.0156" and .007"). I had to scale the chart number for the .007 tool (.0041" offset), but they both worked. I haven't tried a chamfer smaller than the compensation number from the charts. Who knows what that would do...

Like I said before, when I use Visual Quick Code the chamfers are correct. Just the "Intuitive" programming package gives the faulty results.

I don't know why it works this way, but it does and with consistent results. Maybe it is just my machine (early 2008 TL-1). But, you may be getting incorrect chamfers and not know it. If you do big chamfers this little offset may get lost in the noise. But, if you are like me and are just trying to break an edge with a small .010" chamfer, then it is noticeable when the chamfer is 2-3x larger.

YMMV,
Eric

MDI results from my IPS chamfer problem

Ok, here's the MDI result from my chamfer example:
%
O00025
(OD CHAMFER)
T101
G54
G50 S1000
G96 S250 M03
G00 X1.05
G00 Z0.05
G71 P101 Q102 U0 W0 D0.02 F0.004
N101 G00 X0.8876
G01 Z0.
N102 G01 X1. Z-0.0562
G00 X1. Z0.
M30
%

Tool #1 is a 1/32" tnr CNMG turn/face tool. My cut is an OD chamfer on a 1" OD bar, and is supposed to be .025" x 45deg and starts at Z0. I can't really tell what is happening with this...

All my OD tools have a tool nose direction of 3 while my ID tools are a 2.

Thanks for looking!
Eric

Those numbers dont look right, are you measuring your chamfer correctly? That is are you trying to measure the face distance or the distance back from the front face?

A chamfer should be discribed by the distance back from the Z face and the angle.

Charles

I checked my lathe and I don't have any values in tool nose direction in the offsets page. As far as I know you only need the tool nose direction when your using compensation for the tool nose radius. I didn't see any g40, 41, or 42 in the program, but I'm not sure if the G71 stock removal cycle automatically uses tool nose radius comp.

I'd try setting the value for the tip direction to 0 and see what that does.

Can we see the vqc program and compair it to the ips program.

My chamfer is supposed to be .025" back from the front face, or .025"x.025". Someone else had the same question on the CNCzone forum.

Eric

I sent this problem to my HFO. The tech support guy was able to duplicate this issue (incorrect results) on his software simulator with the latest version of IPS. He forwarded this to Haas HQ where they confirmed that it is a known problem. They are supposedly working on it. Since they knew it was an issue in 2008 and it isn't fixed in 2010, I'm guessing it won't be done anytime soon.

Eric

Eric, thanks for keeping us up to date.