Tooltip radius compensation help!

[Predator]

I need to program a cutting path from no. 1 to no.3 as shown in the jpeg attachment, and i understand that G42 should be used to compensate the tool nose radius, but which tool tip number should i use? how should i program it so that i will get an accurate finished product?

[Kiwi]

Normally your cam program would calculate this for you. Just enter the diameter of your cutter and the type. eg Ball nose.
Do you need many of these points or just the four illustrated.
If you require just the four points you could draw the profile with circles tangent to the profile lines. Then calculate the tool path as per the attached drawing.

[Geof]

Do the pictures help? I captured them out of a manual.

I think for your application 8 will be the correct tip number to use.

[Predator]

Thanks for the prompt reply, well there shouldnt be any problems if the codes were generated using cam, however, is there any way to hand-code it correctly?

Geof, the pictures u attached does help, however, the cutting path involves 3 different tool tips and if i am not wrong, G42 only allows using compensation for one tool tip for one cutting cycle..

[Geof]

....Geof, the pictures u attached does help, however, the cutting path involves 3 different tool tips and if i am not wrong, G42 only allows using compensation for one tool tip for one cutting cycle..

How do you get 3 different tool tips? You are not going far enough around the nose radius for the side of the tool to be cutting. You are using the same tool for the entire path in your picture and the toolpath is symmetric, tip 8 works for a symmetric path.

If your angle was steeper you would need to do it with two tools: The front and OD would be done with a tool like that shown for tip 9 and would use tip 9 and the back angle would be done with a tool like tip 4 and use tip 4.

[Predator]

i am actually using a tool holder similar to the tool tip number 3.. not the one in the pic i attached earlier on... the angle of the holder is steeper than the slope i need to cut...

However, my main concern is the tool tip will be cutting the material using one end of the insert on the first slope, however when it reaches the 2nd slope, it will use the other end of the insert to cut the material right?

Pls correct me if my theory is wrong...
was wondering if the 2nd slope will be affected as the cutter is using different sides to cut the material as it moves from the 1st slope to the 2nd..

hope u understand what i mean...

[Geof]

....However, my main concern is the tool tip will be cutting the material using one end of the insert on the first slope, however when it reaches the 2nd slope, it will use the other end of the insert to cut the material right?....

My understanding of the tip 8 tool compensation operation is that the controller corrects for the nose radius on both slopes. It takes the tool past the programmed path by the amount necessary to compensate on the back slope.

If you have a machine that has a good graphics display you can write a little program which follows the tool path first without compensation and then repeats with compensation and you can see from the trace what the compensation is doing.

However, if your tool is actually a different shape you will have to select the tip number for that shape and the path that it follows.

[Kiwi]

Predator:
My pictures are for a milling path.
On further examination I see you need this for a Lathe.
Sorry to put you wrong.

[Predator]

kiwi, its ok, i wasnt clear in the first post, anyway i will try and figure that using a simulator...

[adamant]

Use two tools.

use on like the #3.

and then use one like the #4.


Your TRC values would be 3 and 4

[Predator]

using 2 tools will have no problem with the compensation, however is it possible to use one tool all the way? the tolerance for the workpiece is only 20 microns and it will be much more difficult to control if i were to use 2 tools for finishing...

[Geof]

using 2 tools will have no problem with the compensation, however is it possible to use one tool all the way?...

You can use one tool with a profile the same as you had in your first sketch provided the tip angle on the tool is small enough that the sides of the tool do not touch the angle on either side of the part. This way the tool is only working on the nose radius.

This program does part of a sphere using Tip 8 and a tool like your sketch. It does not go far enough down the sphere for the sides of the tool to touch.


%
N1000 T101
N1001 G00 X1.5 Z1.
N1002 M03 S1800
N1003 X0.6 Z0.15 M08
N1003 G42 G01 X0.3693 Z0.1 F0.01
N1005 G03 R0.5 X0.5057 Z-0.8009
N1006 G40 G00 X1.15
N1007 Z0.18
N1003 G42 G00 X0.3593 Z0.1
N1005 G03 R0.5 X0.4957 Z-0.8009 F0.005
N1006 G40 G00 X1.15
N1023 G00 X2. Z5.
N1024 M99
N1025 (----)
%