[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!

[gar]

070428-0727 EST USA

williamglassII:

If I understand your question correctly, then the procedure is fairly simple.

In the cross-section you have two parallel lines spaced 0.025" apart. This is from (1.450-1.400)/2 = 0.025. Where the two radii meet is 1/2 of 0.025 = 0.0125 .

Now we have a right triangle to solve. The hypotenuse is 0.12 and the long side is 0.12 -0.0125 = 0.1075 . The short side is 0.0533 . For reference the small angle is 26.3843 deg.

In the Z-axis on the lathe the distance between the two arc centers is 2 * 0.0533 = 0.1066 .

The radial or X position of the center of the first arc is 1.425/2 + 0.1075 = 0.8200 from the centerline of the pin. The second arc center position is 1.425/2 - 0.1075 = 0.6050 .

The first arc Z center is -1.0000, and the second is -1.0000 - ( 2 * 0.0533 ) = -1.1066 .

Check my math.

You may need to put a very short straight line at the intersection of the two radii if the controller has a problem with this intersection.

.

[Geof]

Okay, hard way. Although you only need to be a wimpy masochist because it only needs geometry not trig. The two fillet radii are the same.

gar got in a few minutes ahead of me and did the description in words, here is a picture. We did the calculation a bit different; gar mentions angles so I guess he is more of a masochist than me .

[gar]

070428-0905 EST USA

Geof:

I did it first with the Pythagorean theorem, then double checked with COS and TAN.

.

[g-codeguy]

geof and gar- You guys must be wimps! LOL. When I started programming, it was for punch presses. No computer software. Everything had to be figured using 90 deg. formulas. Thank God for computers, hey?

Just joking. From what I've seen so far, you guys know your stuff.

[Geof]

geof and gar- You guys must be wimps! LOL. When I started programming, it was for punch presses. No computer software. Everything had to be figured using 90 deg. formulas. Thank God for computers, hey?

Just joking. From what I've seen so far, you guys know your stuff.

I used an abacus and slide rule when starting. And scratched drawings on birch bark with a piece of charcoal.

[g-codeguy]

I used an abacus and slide rule when starting. And scratched drawings on birch bark with a piece of charcoal.

Say it isn't so!! You can't be older than me. A more descriptive user name for me would have been "OldnUgly".

[Geof]

Say it isn't so!! You can't be older than me. A more descriptive user name for me would have been "OldnUgly".

Okay I admit I stretched things a bit; the abacus and birch bark were a bit of a liberty . The slide rule actually came along years after I finished my apprenticeship in 1963, it was log tables through trade school.

But I agree with your sentiments regarding computers. I have an old old version of Autosketch and now I just sketch things and pick the coordinates off the intersection points.

[tobyaxis]

Okay I admit I stretched things a bit; the abacus and birch bark were a bit of a liberty . The slide rule actually came along years after I finished my apprenticeship in 1963, it was log tables through trade school.

But I agree with your sentiments regarding computers. I have an old old version of Autosketch and now I just sketch things and pick the coordinates off the intersection points.

Geof,

Have you seen BobCAD/CAM V2007 yet??? You may want to update a little bit LOL. With the right Software you could Create some Pretty Scary Parts

You know the ones I'm talking about. The Scary ones that should be done in a 5 Axis Machine but need multiple Fixtures to be done on a 3 Axis Machine.

BTW: You guys might be 100years young but at least your not CRABBY OLD SENILE GRUMPS set in Ridiculous Outdated Ways of Machining..... LOL !!!!!

[Geof]

Geof,

Have you seen BobCAD/CAM V2007 yet??? ....

If I ever do get involved with CAD/CAM it will probably be ONECNC, sorry.

The only thing that discourages me is that no matter what anyone says the learning curve is many months, I don't even use a CAD program so I have to start from the very bottom. It seems a bit pointless to spend the time because I don't need it for the parts we make and if I did I would hire someone.

[g-codeguy]

Okay I admit I stretched things a bit; the abacus and birch bark were a bit of a liberty . The slide rule actually came along years after I finished my apprenticeship in 1963, it was log tables through trade school.

But I agree with your sentiments regarding computers. I have an old old version of Autosketch and now I just sketch things and pick the coordinates off the intersection points.

Hey, I remember log tables! Slide rules too. Think calculators were just coming out.

Most of my programming is done manually, but (being lazy) I use MasterCam so I don't have to figure trig. Layout my rough end point and use Analyze. Company wants me to change and do everything on MasterCam so about anyone can walk off the street, find the part in DWGS, change post for proper machine, and output a good program. No thinking involved! They will probably make twice what I am, too. :violin:

[tobyaxis]

If I ever do get involved with CAD/CAM it will probably be ONECNC, sorry.

The only thing that discourages me is that no matter what anyone says the learning curve is many months, I don't even use a CAD program so I have to start from the very bottom. It seems a bit pointless to spend the time because I don't need it for the parts we make and if I did I would hire someone.

You know where to find me if you need CAD/CAM work.

BTW: I know a few people with ONECNC and they don't seem to get any Tech Support. Personally I don't know why.

As far as learning curve, Geof I'm teaching a 64 year old guy BCC V21 and V2007 at his shop. He makes Aircraft Parts for Boeing, Lockheed, and Sikorsky. This guy is having a blast learning all the stuff I'm teaching him. He is one of a kind.

Personally because he is so cool I cut my price in half because he teaches me stuff too. One hand washes the other.

Cheers!!!!!!!!!

[g-codeguy]

If I ever do get involved with CAD/CAM it will probably be ONECNC, sorry.

The only thing that discourages me is that no matter what anyone says the learning curve is many months, I don't even use a CAD program so I have to start from the very bottom. It seems a bit pointless to spend the time because I don't need it for the parts we make and if I did I would hire someone.

I can't help but think that it wouldn't take long for a man with your knowledge to learn a CAD/CAM system. There is one minor problem, however. Getting a software program to post out so that it looks just like one of your manual programs DOES take time. At least for some of us slower guys. Even then you will find that there will be instances in which you can't make the post put out exactly what you want because of the way the software works.

[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.