[Un4givn]

Hi,

I recently got to work on a job that was too big for my HAAS VF4, but I soon got around this with a 4th axis that i put flat on the table so that it rotates on the Z axis. Because the job is a big round ring I could program it by hand using only the A, X and Z axis, leaving the Y axis out because the job would crash into the machine.
This went well for a while until I opened up a new drawing the engineer gave me. It wasn't round any more...well, almost round except for a few places along the circle where there were simple profiles.
Now I know it is still possible to cut it using only the AXZ axis, the problem is I can't program it by hand, it's gonna be way too complicated for the limited amount of time I have.
After trying long and hard on CAMworks, I couldn't get anything done, using 4 axis machining turns the cutter to cut perpendicular to the surface I'm cutting. All I want is to cut a contour without using Y axis. I tried MasterCam too, no go there also. I can't imagine that I'm the only one who ever wanted to cut in this way, so that means I must be missing something...Could anyone help?

[Kiwi]

Can you post a sketch of the contour and give the Y position of the tool relative to the centre of your A.
Just trying to understand what you require.

[cncbayer16]

Use a G68 inyour G18 or 19 plane along with your g2 or 3 add a z move for some Favorrrr!

[HuFlungDung]

What comes to my mind is that you'd need something like Mill/Turn functionality because you've got polar coordinate programming to deal with. OneCNC now has this sort of functionality available, obviously meant for lathes with a live 4th, but I can at least imagine hacking a post to make it run on a mill

[Un4givn]

Here is a rough sketch, it's bad quality but you can get the general idea. Y axis stands still on Y0.0 in the center of the job. That's also where my A axis rotates.

I know it doesn't look like much but those curves are critical, and right in the middle of the little profile is a flat part for 35mm.

[Kiwi]

My suggestion would to generate a tool path with G01 steps.
Open NC file with Excel and calculate Angle and X

[Un4givn]

I thought of the same thing this morning while driving to work. That ring you see is 900mm in diameter though, so I'm going to need a way to calculate about 250000 steps to get within 0.02mm between steps. Have you got any idea how I can calculate that fast?

I saw the pic you sent but my excel knowledge is somewhat limited. If that is the answer I'm looking for could you just explain a bit more in detail?

This is the way though, I just need to calculate those coordinates.

[Kiwi]

.....so I'm going to need a way to calculate about 250000 steps to get within 0.02mm between steps.

I saw the pic you sent but my excel knowledge is somewhat limited. If that is the answer I'm looking for could you just explain a bit more in detail?

When the path is on a constant radius, only one line of code is required, but when machining the flats and the small arcs, I believe you need many short movements to maintain accuracy.

The method I'm suggesting has a number of steps to get what you require, but I don't have a 4th axis CAM program to advise using one.

Please supply some details of your drawing and I will supply some code with details on the method I'm using.

[cncbayer16]

I want to Buy a 20" swing lathe (not to require that it is cuts to that dia) just need it to be fadal or the Kentucky thourghbreed, A MAZAK, either way I m a lookin @ all ,, Thanks

[Matt@RFR]

You don't need to make it complicated. Position the tool where needed and feed A until you get to the first radius going into one of the tabs. Stop the A right there and lead out along that radius. Then reenter the cut and interpolate the step without moving A. Reposition so Y is on centerline with A again and keep cutting until you encounter the next tab.

If you're programming manually, just make the above into a local sub and loop it in Z until you're through, then change your D number for that tool and run the finish pass. No biggie.

[Kiwi]

You don't need to make it complicated...........

I like your approach but this may only be possible if the Y travel doesn't crash the job into the machine.

........ leaving the Y axis out because the job would crash into the machine......

[Matt@RFR]

Thanks Kiwi, I missed that part somehow. Those tabs on the part look small so hopefully he's got enough room to move Y by that much. If not, that is one tight fit!

[Un4givn]

Nope, no room, I've literally got 4mm of space behind the job before it crashes in Y. The other problem is that there is a flat spot on the tabs for 35mm.

But I had a stroke of genius yesterday. I drew 120 degrees of the profile(basicaly from the start of one tab to the start of the other) in a straight line by taking key points and using the radius for X and the angle for Y. After I've done that I scaled the Y up to the total length of the profile for the 120 degrees so I could put in the tangent arcs. Then I scaled back down to 120 mm. I hope this makes sense so far...

Now all I need to do is program this weird looking straight profile and change all the Y's to A's. Some minor tweaks will need to be done in the program but that's no biggie, and I can use this in a subprogram to cut the whole 360 degrees.

I'm busy double checking everything but so far it seems as though it's gonna work. Here's a pic.

[Kiwi]

Attached is a program to calculate the Angle and the X dim for half the flat only.
If this agrees with you figures and is of any use I will modify as required.

[Un4givn]

Cool I'll have a look at it and compare it to the solid and the method I came up with. Quite a handy little program.
Does the method I described make any sense to you?

[Kiwi]

..........Does the method I described make any sense to you?

Sorry, no I haven't seen the light yet.
The constant radius is no problem and if your code/calculator code is good for the flats, how important is the transition from the flat to the curve?

[cnc2]

Attached is a program to calculate the Angle and the X dim for half the flat only.
If this agrees with you figures and is of any use I will modify as required.

#####OUT OF TOPIC WARNING######

Hi Kiwi !

I'm a student in the computing & networking field & i'm impressed by your program i also got a few questions:

1) Which programming language did you use ?
2) How is the G code generated ?
3) Is there any G code programming library or you wrote all the routines by yourself ?

Guys excuse me going out of topic.

Thanks !
cnc2.

[Kiwi]

1) Which programming language did you use ?
2) How is the G code generated ?
3) Is there any G code programming library or you wrote all the routines by yourself ?

Hi CNC2
1.The program is written with VisualBasic6
2.The code is generated by looping though the arc range while calculating the positions which are added to a String.
3.All my own work.
I've written a number of programs like this one to generate code.
I prefer to generate code this way than to write a GCode macro to run on the controller.

[cnc2]

Thanks for the reply Kiwi !

Great work man, how long did it take to program the conversion of the output to G code ?
Does it require a full mastering of Gcode or it requires just a conversion table ?

Which way should i follow to reach that level of programming ? (do i need to know about graphics or you just use a circle function for a given range and then call a line function for another range)

Excuse my last question, sometimes things are more complicated than they look like & sometimes it's of childish simplicity but it remains hidden to the naked(newbie) eye.

Sorry guys.

Thanks !
cnc2.

[Kiwi]

...how long did it take to program the conversion of the output to G code ?.....

The VB loop output is the angle and the X dimension so only the 'A' and 'X' need to be added to become GCode.

...Does it require a full mastering of Gcode or it requires just a conversion table ?

As the output is made up of 'A' rotations and 'G01 X' movements there is very little GCode knowledge required....

...Which way should i follow to reach that level of programming ?....

For this exercise you need to understand where the tool should be as the disc rotates so a basics of trig is required. I do a drawing with CAD to confirm the figures.