tool nose radius comp

[joe1970]

Help Please,
I have always used g41 or g42 in turning to get my angles and radii to come out to print. However I have purchached an older machine which does not have tool radius comp option.

I seem to remember in years past a formula or constant to add (or subtract) in x and z for an angle or radius to come out to print. Does anyone know the formula or trig or constant for diffrent tool nose radii??

Any help would be greatly appreciated
Thanx

[wjbzone]

It's not a simple formula to cover all cases because you have different touch off points on your tool depending on direction of machining and ID vs OD.

I approach it like I am programming the center of the tool on a line that is offset by the tool radius. Then shift the X and Z in the direction of your touch off point.

Take a look at this attachment.
http://www.cnczone.com/forums/attach...tachmentid=392
in this thread.
Lathe programing help

At least its a start.
Bill

[bbailey]

Hi,

Send me a personal message with your e-mail and I will send you an Excel file that may be able to help.

[cnc wizard]

Here ya go...

Xcomp=R-(R*TANGENT((90-A) / 2)

Zcomp=R-(R*TANGENT(A / 2))

R= The nose radius of the tool.
A = The angle your cutting. Make sure you use the right angle. It will be the one measured from the "Z" axis.

Example: if you are cutting a 60 degree angle using a .015 tool nose radius.

Xcomp= .015 - (.015 x tangent((90-60) / 2

Xcomp = .015 - (.015 x tangent (30) / 2

Xcomp = .015 - (.015 x tangent of 15)

Xcomp = .015 - (.015 x .2679)

Xcomp = .015 - .004

Xcomp = .011

Program the above formulas into a programmable calculator and your on easy street!

[joe1970]

thanks Wiz a big time saver!! now I don't have to go to the cam system for a simple face and turn operation with an angle or radius .
Joe

[madonno]

Hi. I just uploaded an Excel spreadsheet that calculates the compensations.
I hope it's correct!
Here's the link with the triangle that shows where the angle and the axis are.
click here

[rod88]

This is great to have, thank you I do a lot of manual programing with out cutter comp. Do you have any help with how I can get it to work to go from a radius into a 45 degree angle? say a .031 tool nose into the angle

[madonno]

That's tricky. I did it once and it took me quite a while to figure out how to calculate the difference between a .016 and a .031 radius. I have to check in my notebook at work tomorrow. Maybe I can also create another Excel spreadsheet for that.

[madonno]

Funny thing happened yesterday at work. The thread relief had a big radius (twice the width of the grooving tool) and the programmer didn't rough the radius at all. So I accidentally calculated the required X-Values for a Z-movement into the radius correctly!
So the radius was R.1106 and it started at X.5336 and Z-.8734 and ended at X.7548 and Z-.984.
So with my .063 grooving insert I wanted to rough it in 2 steps. I added .055 in to the starting point in Z (.8734 + .055): Z-.9284
The X value I calculated like this:
I took the root of Square R (.1106) - Square Z value (.055) and subtracted that from R. Multiplied that by 2 and added it to the start point in X (.5336)

I accidentally mixed up the Pythagorean theorem!