Eccentric turning

[littlerob]

Need some help guys, I am quoting a job that requires eccentric turning on both ends, I have the machine capacity, (X, Y, Z, C, W, . But I cannot figure out the right toolpath or chaining method to do this. I am using X2 and this job may be the right push for the owner to buy maintenence (hopefully). But can the toolpath be found in X2?, and if not can it be found in X6 or 7?

 

Thanks, Robert

[htm01]

you need to mill that or have a 4jaw or buck chuck to turn a dia. off center

[GoetzInd]

Edit: Not my video.

I wrote a macro to do this once and posted how somewhere. I'll try and dig it up. Otherwise, you can use a 5axis path and lock it to fourth. However, depending on your machine processing speed, all the code may slow down you effective SFM.

Mike

[littlerob]

Edit: Not my video.

 

I wrote a macro to do this once and posted how somewhere. I'll try and dig it up. Otherwise, you can use a 5axis path and lock it to fourth. However, depending on your machine processing speed, all the code may slow down you effective SFM.

 

Mike

 

 

 

That is exactly what I need to do just without the Y moves, if you can get me the info on the Macro that would be great, the control is a newish (2006) Mazak Nexus so memory isn't an issue, if we gotta go slow, so be it. I just need to know if X2 will give me the code, have lathe level 1 with Mill level 1. I don't see anything 5 axis just C.

 

Thanks again, Robert

[mkd]

if no y axis; just do a c-axis face Endmill path.

last time i did it was ver 9 so x2 is capable

 

 

^^very cool video, BTW^^^

[GoetzInd]

You are going to have to have a major clearance angle on your tool and have the geometry only slightly off center for it to work without using Y. Do you have a file or screenshot of what you are trying to do?

 

Mike

[mkd]

it gets interesting at the 3:00 mark...
and whoever is driving the forklift needs to stop!

[Greg Williams]

^^ Nice vid that one ^^

 

It uses a small macro

 

OCALL

T020202

M110

M808

NLP1

ZZ1=0

PTC=0.1

G94 M146

G00 X400 Z0

G138

G0 X400

FF1=95000

XX1=111.5/2

G17

G0 Y0 C0

X=XX1

NLOOP

ZZ1=ZZ1-PTC

M15

G01 C180 X=XX1 Z=ZZ1 F=FF1

ZZ1=ZZ1-PTC

G01 C0 X=XX1-6 Z=ZZ1 F=FF1

IF [ZZ1 GT -13] NLOOP

G00 X400

G0 Y0 C0

G136

G00 X400

M109

RTS

 

You can also do this with a 5 axis curve toolpath. You need to be careful if there is a roundness tolerance, This method is really only good for roughing.