Haas IPS chamfer problem

[ProneKing]

Hi,

On my TL-1, when I try to do a chamfer with the intuitive programming the size is too big. This applies to both ID and OD 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 size of chamfer. 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.

It took me a while to remember how I did this as I didn't use my lathe at all for about 1.5 years. When I tried doing my first sample chamfer last week 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 tables 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...

When I use Visual Quick Code the chamfers are correct. Problem with VQC is that chamfers are part of a bigger operation and I just want a chamfer. It is 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.

I've got the correct tool nose radius in both my offsets page and on the IPS screen. Nothing in wear offsets.

Any idea why my lathe works this way? Any way of fixing it? I'd really like to just plug numbers into IPS and run...

Thanks,
Eric

[Donkey Hotey]

As posted on the other forum, post up the G-code that IPS is generating and lets have a look at it. Putting in the tool nose radius is only part of it. You also have to use tool nose compensation.

Then there is one other messy little bit: even if you are using TNC, are you using the right cutter direction? Remember that your TL-1 is programmed upside-down from the examples in the book. Which direction is your TNC? If it's backward, the TNC could be exaggerating the cut.

[ProneKing]

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

[Donkey Hotey]

I haven't tried my TL-1 for comparison but, this is what's going on:

There is no actual tool nose compensation going on but, it looks like IPS is trying to do some kind of compensation based on the radius and direction loaded into the offset table.

In Solidworks, I laid out the dimensions you wanted as well as the g-code you gave above. It looks like the tool nose radius is off by about half (the actual tool would need to be just about double what you input to give you the proper chamfer). It's not exactly half and that still puzzles me.

Just so we're clear: when you say 0.025" chamfer, you mean 0.025" measured 45 degrees to the shaft, correct? Not a 0.025x0.025" chamfer? Different people mean different things and I'm never sure without analyzing their CAD model.

[Geof]

.....Just so we're clear: when you say 0.025" chamfer, you mean 0.025" measured 45 degrees to the shaft, correct? Not a 0.025x0.025" chamfer? Different people mean different things and I'm never sure without analyzing their CAD model.

Different people should not mean different things. Is this another case of a convention from manual drafting being lost? Chamfers should always be measured by the distance back from the corner that is being chamfered, not on the hypotenuse.

[Donkey Hotey]

Different people should not mean different things. Is this another case of a convention from manual drafting being lost? Chamfers should always be measured by the distance back from the corner that is being chamfered, not on the hypotenuse.

I hear ya', Geof. I've watched machinists measure on the hypotenuse and had this discussion. I don't know what they mean anymore. Because of the ambiguity, I don't actually use chamfer call outs anymore. I either use "break sharp edges", detailed dimensions or I put a loose dimension radius.

[ProneKing]

My chamfer is .025"x.025".

I also laid this chamfer out in Solidworks and it looked like about a .038"x.038" chamfer resulted. Not too far off from my .040" guesstimate.

Eric

[ProneKing]

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

[CMJacked]

59% of your TNR is your answer for a 45 deg angle...
A 2" bar with a .25 a 45 deg chamfer...
G01 X-.0624 Z0
X1.4634
X2. Z-.2683
Z-5.
It's actually .5858