[williamglassII]

I am looking for information on how to find the X and Z cordinates when programming a blend or radius for a turning center. I have the equations in the Machinery's Handbook, and understand them, but cannot figure out how to use them in referance to our shops prints. For instance. I have a pin that has two OD's. One is 1.400 +- .002 to 1.450 +- .005 the radius starts 1.000 from face of pin and the pin is 4.000 inches long. It has blended radii between the step of r.120 each (G3 to G2 respectivly). I am told that I need to find the Chord/Chords to figure out how to program the z and x cordinates (absolute programming) but with this information I don't know how. The equations I have tell me that I need to know two of these things to find this... The radius (which I know), the chord (which I need), the angle, the length of the arc, or the hight of the arc from the chord. I am using a Cincinnati Hawk with an Acramatic 2100 control 'Siemens'. The above example given was only an example, I'm trying to understand the concept of programming partial arcs without the use of a program. Although most programs i've seen need two of those numbers to figure out the arc too. I hope any of what I said makes any sense to someone, any help would be greatly appreciated. My e-mail is [email protected]. Thanks.

[tobyaxis]

I'll try to make you a drawing of what you need and post a pic later. One thing that you have to remember with Lathes is that your working in Diameters not Radii. So with that said everything in Z is Double in X.

Also you will need to use Tool Tip Compensation unless you want to spend wasted hours fudging around with your program to get the geometry on the part correct.

In the Tool Offset Geometry Page you will see X Z R T

X= Geometry Position part Center Line
Z= Geometry Position Face Z0
R= The Radius of the Tool Tip Insert ANSI CNMG432= .0312 Tip Radius
T= Tool Tip Designation 0-9 (for an O.D. turning tool this would be set to "3" and I.D. Boring Tool it will be set to "2") There should be a Chart in the Programming Manual

G42 is for O.D Turning Toward the Spindle
G41 is for I.D. Boring Toward the Spindle

Example a 1 inch diameter with a .1 45 Degree Chamfer is as follows.

O0001
G0G40G80G99M5
G28U0W0M9
M1

N1(TURN)
T0101M8
G50S2000M39
G96S500M3
G40G0X1.125Z.1
X0
G42G1Z0F.006
X.8
X1.0Z-.1
Z-1.0
X1.125
G40G0Z.1M9
G97
G28U0W0
M30


Example with a radius of .1

O0001
G0G40G80G99M5
G28U0W0M9
M1

N1(TURN CNMG432)
T0101M8
G50S2000M39
G96S500M3
G40G0X1.125Z.1
X0
G42G1Z0F.006
X.8
G3X1.0Z-.1R.1
G1Z-1.0
X1.125
G40G0Z.1M9
G97
G28U0W0
M30

Hop this helps.

[williamglassII]

I think I understand. My company thinks that g41 and 42 are evil so the nose comp is programmed by hand. That's ok, it's made me very quick and good with fractions to dec. :-) I think this is stupid, but I'm not high enough or willing to change thousands of programs to add this. I'm still a little confused on the radius though. I don't have to know what the chord of the arc is? Chamfers I have pat. 45's are easy double X,Z. All other angled chamfers I think are found by (Side "B" / tan of angle "b"), then just take the numbers and make them X and Z moves. Thanks again.

[tobyaxis]

I think I understand. My company thinks that g41 and 42 are evil so the nose comp is programmed by hand. That's ok, it's made me very quick and good with fractions to dec. :-) I think this is stupid, but I'm not high enough or willing to change thousands of programs to add this. I'm still a little confused on the radius though. I don't have to know what the chord of the arc is? Chamfers I have pat. 45's are easy double X,Z. All other angled chamfers I think are found by (Side "B" / tan of angle "b"), then just take the numbers and make them X and Z moves. Thanks again.

G41/G42 are way better than the extra math that will have done without them, LOL. A Program should Match the Print to make edits easier plus less programming/tweaking to get it right the first time.

Believe me on parts like this for Lockheed Martin you better have the Right Geometry because there are 600 shops out there that are waiting for you to make a critical mistake.

G41/G42 = Friends :cheers:

[Geof]

You have to be a masochist to choose to do it by calculation . Get a cheap and simple 2D drafting program; I use a version of AutoSketch I bought in 1987. Just draw your diameter lines and the two circles that correspond to the fillet radii, move them around until the circles blend then zoom in and read off the coordinates.

In the picture I put Z zero at what I think is your 1" point so these coordinates have to be shifted to suit. The X are part coordinates, you can figure the tool nose rad correction if you're not permitted to use tool comp.

Note in the picture the circles don't blend but on the AutoSketch screen they did.

[williamglassII]

I guess I am sort of a Massocist, I really wish to know how to trig/Geom. it out. I guess I feel if I can do this, I Really know how to program it. :-) Peac to all and thank you to toabyaxis (my friend the evil machinist) and geoff (Dat's too easy!! Espc when my shop does everything the hard way!) P.S. If either of you need a setup operator, I would be glad to fill that position!!! (Not an ad, just a desperate act!) Peace to all and have a great weekend.

[williamglassII]

WOW, You have helped me the most!! Thanks!

[j-radkemachine]

hey man... it'd be great if you could come over & teach me how to use my bob-cad.... had it for 2 years & haven't cut a chip using it yet.

[g-codeguy]

hey man... it'd be great if you could come over & teach me how to use my bob-cad.... had it for 2 years & haven't cut a chip using it yet.

Where do you work? I am on the PA/NJ border. Never used Bob-cad, but there shouldn't be that much difference between any of the cad programs.

[tobyaxis]

Where do you work? I am on the PA/NJ border. Never used Bob-cad, but there shouldn't be that much difference between any of the cad programs.

BCC is a lot different than than other CAD/CAM Softwares. My Question is what version is j-radkemachine using????

(hey man... it'd be great if you could come over & teach me how to use my bob-cad.... had it for 2 years & haven't cut a chip using it yet.)

j-radkemachine, you can find help for BobCAD/CAM on CAD/CAM Trainer, Sorin Nenu's website. He is the Official Trainer for BCC.

BTW he has Free Video Tutorials on that site for Versions 19-21 and a few of us are using V2007 that we can help you with too.

http://cadcamtrainer.com/forums/index.php

Cheers!!!!!!!!!

[g-codeguy]

For .03R on part using a .03R tool.

X2.88Z-.01 (Start Position)
G3X3.Z-.07R.06 (End Position)

No need for a CAD on this part. You could have it programmed by the time you lay it out in CAD. Your program would have run had you used R.06 even though the Z-value is .0005 off. At least it would have on the machines I program for.

[j-radkemachine]

drwgs. on birch bark w/ charcoal.... at's funny right der

[j-radkemachine]

this is actually one of the more insightful threads i have read on here... simple but some good basic info.

wish i could find more like it ( w / calcualations of arc / arc intersections )

[Kiwi]

williamglassII
Here is a simple VB program which you may be of some use.
Check the output figures as I'm not familiar with Lathe programming.

[kperk12345]

with chamfers I just use tnr error = tnr(1-tan(ang/2))

[p8md]

I am trying to program a lathe cutting the face and OD with a blended corner radius. I'm using G2/G3 and I have figured out my end point in CAD but the cutter is taking the long way around the radius giving me a "hump" instead of a blended radius (see pic with red radius). How can I fix it?

Thanks,
Mark

[Geof]

....the cutter is taking the long way around the radius giving me a "hump" instead of a blended radius (see pic with red radius). How can I fix it?

Thanks,
Mark

When you use G02/03 with R normally a positive R value tells the controller to do the short path, i.e. an arc that covers less than 180 degrees, and a negative R tells it to do the long path for an arc that covers more than 180 degrees.

[p8md]

OK... so what if the radius is a positive value and still goes the long way.

[Geof]

OK... so what if the radius is a positive value and still goes the long way.

Have you tried both positive and negative?

Your measured 0.100 radius from a .03 tool nose and R 0.130 is correct without tool compensation which you do not mention.

I think you may get the hump if your tangent points are not correct; what is the complete code leading up to, around and away from your corner?

[p8md]

Well, it wasn't doing exactly what I said...

When I tried to create a .030" corner radius with .030" nose radius tool, it was doing the "loop" as described above. But when I also try to create a .130" radius with a .030" nose radius tool, it measures .100" (.030 off) and has the hump appearance. Any ideas what I'm missing?