Machining a curve with just C and Z (lathe application)

[fordav11]

Is it possible in Mastercam to machine a curve on the side of a part using just C and Z (i.e. on a lathe with live tools but no Y axis)? I do it on my machine by taking cuts roughly where they should be then adjusting it slowly until I get what I need (deburring holes or slots etc) but it would be nice to have Mastercam work it out for me so the curve is more precise and smoother

[JIMMY]

I don't know the answer to this 1 but I'll try to find out

[txcncman]

I see no reason this is not possible. Use Toolpath - Mill - Contour. Then in Parameters, Rotary Axis - Axis Substitution. Set Rotary Diameter and Unroll. You should get some G-code that looks similar to this:

G18
M23
G0 G54 X1.25 Z.0313
C11.937
G97 S2500 M51
X.95
G98 G1 X.75 F6.16
C7.162 F941.31
Z.0302 C5.928
Z.0271 C4.775 F871.02
Z.0221 C3.784 F747.15
Z.0156 C3.024 F574.85

[fordav11]

hmmm, that looks promising.
Can I get a bit more detail?
Maybe if I supply some real numbers....

5/8" hole drilled at Z-1.059"
bore is dia 2.43"
tool is a 45 degree chamfer tool (90 degree included angle) dia 7/16" (11.1mm)
I'm chamfering the inside of the hole. the chamfer is around 0.040" so the outer diameter of the chamfer circle is 0.705"

Here's the code I hacked up.....

G00 C0 X2.90 Z-1.059
G01 X2.200 F30.0
M15 (= C clockwise rotation)
C6.0
M16 (= C anti-clockwise rotation)
C5.5  Z-0.991
C5.0  Z-0.969
C4.0  Z-0.944
C0    Z-0.915
C-4.0 Z-0.944
C-5.0 Z-0.969
C-5.5 Z-0.991
C-6.0 Z-1.059
M15
C-5.5 Z-1.127
C-5.0 Z-1.149
C-4.0 Z-1.174
C0    Z-1.203
C4.0  Z-1.174
C5.0  Z-1.149
C5.5  Z-1.127
C6.0  Z-1.059
M16
G0 C0
G0 X3.0

And see pic attached

Can it generate something similar but with say 0.5 degree increments and all the way from 0 degrees to 6.0 degrees (or whatever the software determines is the maximum degrees required)?

[txcncman]

What version of MasterCAM? I get tired of making up files with X3 and then some guy whining "I only have 9."

[txcncman]

Oh. Wait. You are trying to machine this on the inside? How do you propose that the shank of the tool will not interfere with the Z+ and Z- sides of the upper hole? Do you have a reduced shank tool adequate to do this? Why not just use a small back facing boring bar from the top side?

[txcncman]

Anyway, to make the geometry for a tool path you will have to make a cylinder surface at 2.430 diameter. Then make a 0.703 diameter circle at Z-1.059. Then project this circle onto the surface of the cylinder. This projection will be your tool path. Then use the steps described above.

[fordav11]

I mostly use X4 but I also have access to V9 and Mastercam X
Thanks!

I'm only machining one hole at a time. I'm coming in from the top and chamfering the top hole underneath. The tool has a 1/4" shank so plenty of clearance. Mastercam calls this tool type a dovetail cutter but it's actually a threading/grooving tool. It works great but the tool path is not as smooth as I would like
The specific tool is shown below. Its a Sandvik Coromant Corocut MB series grooving tool fitted with a 90 degrees insert specifically for chamfering. Other grooving/threading inserts are available.....
http://www.sandvik.com/sandvik/0110/...3FOpenDocument

[txcncman]

@ford - I will attach the files I came up with. I did not get real picky on setting depth, etc. Just enough to show it can work. I will let you play with the numbers and the tool to get what you need.

Step 1: Set MasterCAM up with Lathe selected
Step 2: Create Circle 0.625 diameter at D=0.000, Y=0.000, and Z= -1.059
Step 3: Change WCS, Cplane, and Tplane to Right Side
Step 4: Create Circle at X0.000, Y0.000, and Z0.000 diameter 2.43
Step 5: Create Surface Extrude 2.000 length in direction of 0.625 diameter
Step 6: Switch to Wireframe
Step 7: Change WCS, Cplane, Tplane back to Top
Step 8: Project 0.625 diameter onto Surface (Cylinder) that was created
Step 9: Toolpath - Mill - Contour - Rotary Axis - Axis substitution - Rotary Diameter 1.215 - Unroll - Tolerance 0.001 -- Set 3D Chamfer - Set Lead In/Lead Out - Set Depth 0. - Set Compensation - Etc.

Sample of G-code output:

G0 G54 X4.1449 Z-.8989
C90.683
G97 S2139 M51
X3.8449
G98 G1 X2.275 F8.56
G42 Z-.7739 C90.48
Z-.7714 C90.409 F213.04
Z-.7697 C90.237 F383.77
Z-.769 C90.004 F426.14
C89.806
Z-.7691 C89.613
Z-.7693 C89.42
Z-.7696 C89.227
Z-.7699 C89.033
Z-.7703 C88.838
Z-.7708 C88.641

[fordav11]

Nice

hmmm this is getting quite complicated.

I made some adjustments to the tool spec (its essentially a 7/16" dia. flat bottom chamfer tool where it can cut only near the largest diameter... see my tool pic in previous post) and I'm not using G41/G42. The Z values are getting closer to where they should be
See attached.

I have some questions.....

1. How to set the center of the 0.625" hole at 0 degrees on the C axis?
The center of the hole is set at 90 degrees now?

2. The Z values are still moving a bit too much off center (Z-1.059). I guess it can be controlled with the X depth but where is the X depth setting?

3. Is it possible to have the tool roll around the curve of the larger (2.43") diameter also? i.e. compensate in X while moving in Z/C. I've found when cutting larger holes on smaller diameters that X needs to move minus otherwise the tool cuts a bigger chamfer when the C axis is at its maximum plus/minus value. I hacked in some X values to compensate for that but would be nice if Mastercam can work that out too.

Thanks for your assistance so far

[txcncman]

I have never done this internal chamfering in practical application. This was produced all on theory that I was sure it can be done in MasterCAM. You can try changing the method from 3D chamfering to 2D. Or don't chamfer at all and just do a 3D tool path and adjust offsetting. Try not using unroll and see what you get. Unless you spend hours and hours in a MasterCAM class, the only way to learn it is trial and error. Even in most classes, you will still end up with trial and error. I have probably spent near 2000 hours with MasterCAM and I still do not know all of the "tricks". I do know that I have always been able to get MasterCAM to output the G-code I expect it to to successfully make parts.

And, yes. Machining and CNC programming can be quite complicated. Most machine shop owners "don't get it." They want to pay programmers and set up people the same as the operators. Not to mention most of the people "wanting" to be programmers and set up skimp on their educations.

[fordav11]

I gave up worrying about shop owners 15 years ago. Wannabe's.... well, we have a couple in our office as programmers. I usually just delete whatever they did and do it the right way. Not had a problem so far
Those without the skills but wanting to be CNC Programmers / Machinists / Setters will never be programmers / real machinists without real machining qualifications and technical knowledge. I like to call them 'button pushers'. There are many at my work. Some of them call themselves qualified tradesmen but they probably got their license out of a cereal box or paid the required fee in India

I never said CNC Machining / Programming in general was complicated... at least not 2D/2.5D
3D is where it gets complicated :/

Without 'unroll' X values are added (looks promising!) but the C/Z values are too weird to be useful. I guess all of this 3D stuff really needs a Y axis to do it properly. a C/Z axis set-up is just a poor man's Y axis

I think the easiest way to do this is just cut a 0.705" circle and skip the chamfering b.s. entirely since the tool/tip angle does the chamfer anyway. I can handle that part now thanks to your example.

So do you have any idea about how to place the hole (0.625" circle) at 0 degrees on the C axis?
I guess I can just subtract 90 from all generated C values