[Ya-Nvr-No]

Is it possible to setup MadCam to use a 4th axis rotary table sitting on the "XY" table of a vertical milling machine. I'd like to side cut some multi lobe Cam profiles.

And is it possible to setup MadCam to use the lathe Servo Spindle axis "C" and using a "Y" axis Servo Spindle, mill in both the "Z" axis and the "XY" axis?
Cutting and drilling on the OD "Y" axis
or Milling and drilling on the face in "Z" axis by rotating the "Y" Servo Spindle 90 degrees.

"B" axis Servo Spindle sets on the cross slide "X" axis?

Don't seem to have any luck with the "Z" axis and "C" axis working together.

Any help would be great, Thanks
www.yanvrno.com

[subnoize]

Nevermind, I miss understood what you were asking.

[Ya-Nvr-No]

With over 100 views and No responses, Does that mean it is not possible to setup MADCAM to use the "C" rotary axis with the "Z" linear axis?

[svenakela]

With over 100 views and No responses, Does that mean it is not possible to setup MADCAM to use the "C" rotary axis with the "Z" linear axis?

Well, I think I understood half of the OP... Of course you can add a rotary axle, it's just a fourth axle in a 4-axis machine. You need a 4X license to create full simultaneous tool paths.
If you want to run your lathe as a flipped CNC it's up to you to make it happen in the lathe, make sure the controller can behave like you want and you probably need to write a post processor that fits your needs. MadCAM, doesn't really care what your machine looks like.

[Ya-Nvr-No]

Thanks for helping.
I have full 5 axis multi version.

Using 4-axis functions (simultaneous 4-axis)
Origin(0,0,0) Direction(0,0,1)
I get the message:
Error! The spindle axis is parallell to the rotary axis.

(and yes the spelling is as shown)
Based on what you posted, Why is this an error?
Is it because of my post processor is not written correctly?
If so what am I missing in my post?

Or Is it because for some reason, I have madCAM in three separate menu options but only one Toolbar?
seems like everytime I upgraded it creates a new menu option.
Only shows one checked in the plugin options checkboxes.

Thanks again,

[Ya-Nvr-No]

Attachment 222880
(just a quick sketch I created to see if I can develop a 4 axis post setup)

can manage to pick a 5 axis post so I could show the C axis rotation
Just can not get the tool to work only in the Z to C axis.
Always wants to use the end of the tool and not the side.
No luck editing the post to get the tool and "C" rotary axis to machine in the same alignment using the side of the tool and rotating the "C" only.

[Ya-Nvr-No]

Attachment 222886

setting in the 5th axis options
if I set the spindle axis to .0001,.0001,1
I get past the error of alignment
but the issue, is it does not rotate around the C axis then.

[Ya-Nvr-No]

Attachment 222898

Attachment 222900

using the spindle out of alignment trick, I can manage to get it to rotate in "C" in the 5th axis mode using the "5-axis Trunion_Machine" option
just not found a way to do it in 4axis mode and the "C" axis and "Z" spindle axis in alignment.

[svenakela]

Have a look at this post.
http://www.cnczone.com/forums/madcam...ml#post1425340

[Ya-Nvr-No]

Thanks for the link, I like it for clarification of a few questions I had on 5 axis setups, but still does not address how to setup a 4th axis "inline" with the spindle. I can lie to it to get it to work for the most part, but that does not seem like a great alternative to setup a 4 axis system.

I am getting closer but still have to fudge the "Z" axis spindle direction to beable to generate tool paths.

[ShapeShaver]

This is how to setup madCAM for your machine.

1) Click on madCAM options from the madCAM toolbar.
Attachment 224372

2) Select a 5-axis table/head machine and click OK to choose this kind of machine.
Attachment 224374


3) Attachment 224376Click on madCAM options again and select 5-axis Custom and fill in the vectors for the 4th and 5th axis as in the picture below.
Attachment 224378


You will not use the 4th axis because its fixed, but as long as you make 4-axis toolpaths from your c-axis, the spindle will be perpendicular to the Z-axis which will simulate and post process correctly anyway.

4) Next thing is to edit the post processor, but you don't have to do that because I have attached a new Mach3-5-axis post processor with this mail, but I show you anyway so you know how it works.
:
:
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*AXIS_4_CHAR*
B <== This is the character for the 4th axis. It doesn't matter if setting this, because you will not use it.
*AXIS_5_CHAR*
C <== This is the character for the 5th axis and you will use it as your 4th axis.
*CUTTER_REFERENCE*
TIP
*TOOLPATH_OUTPUT*
TRANSFORM
*RAPID*
G00"x""y""z""b" <== These are the variables for the output. For a 5-axis machine the output would have been G00"x""y""z""a""b". If removing "a", it will only output x,y,z and your c-axis.
*END_SECTION*
*RAPID_APPROACH*
"x""y""z""b"
*END_SECTION*
*RAPID_RETRACT*
G00"x""y""z""b"
*END_SECTION*
*APPROACH*
G01"x""y""z""b" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x""y""z""b" F"feed"
*END_SECTION*
*CUT*
"x""y""z""b"
*END_SECTION*
:
:
:

You can copy the attached post processor Mach3_C-4-axis.txt to your computer and then select it as your default post processor from madCAM options.



If you still are having trouble, please let me know.
I am not sure if the c-axis rotation should be in clockwise positive direction or not, but I will help you to reverse the direction if needed.

Regards,

Joakim Möller

[ShapeShaver]

Ya-Nvr, I also have a rotary table on my XY and that was the emailed instructions I received from Joakim on how to set it up. I can't attach a file so you will have to manually change your post processor to match the part shown above.

One thing to be aware of however, is that my machine is a gantry and my A axis is slaved to my Y. So you will have to figure out the neccessary changes in the post processor.

I hope that gets you what you need to solve your problem.

SS

[ShapeShaver]

Ah, i figured out how to attach a file. Here it is.

[Ya-Nvr-No]

Thanks that helped to understand a little about the need to edit the post.
But I'm still fighting how to setup the 4 axis settings
I've circled a few issues in this screen capture.

Attachment 224534

How do you get the revolution graphics to setup correctly?
Attachment 224536
Attachment 224538


looks good in the x or y but how do you get it to work in Z
just gives me an error of axis parallel. Why cant they be?

[ShapeShaver]

I don't think you can have both your rotary direction in Z, and your spindle tooling oriented in Z. Didn't you say you were going to come from the side and machine the sides with the tool horizontal? If that is the case, try to set the spindle axis direction to X or Y and see if that works.

Also try making the spindle origin off center from the rotary origin so they are not co-axial. I don't think madCAM likes that.

[Ya-Nvr-No]

I have two separate applications needs, One is a standard gantry router style machine that Id like to be able to add C axis capabilities only using (Y or X),Z and C axis. Size and accuracy is always around the centerline of the rotary C axis base.

The second is a lathe with a spindle on a Y vertical axis angleplate mounted on the X axis crossslide. The B axis spindle that can be set at 90 degree angles to the axis. What Id like to beable to do is drill holes inline with the spindle axis but positional. Having C axis spindle positioning I can drill or mill any location on the face of the part. Or rotating the Y axis spindle head I can drill or mill on the OD of the part. The B axis spindle also has positioning capabilities.

I can generate code and then just edit it to suit my directional needs but I'd like to beable to setup MadCAM post to handle this setup.

Might be easier to visualize with a photo;
Photo shows the lathe with the Spindle at 90 degrees to the Z axis.
Attachment 224636

[ShapeShaver]

To set up your C axis you can follow the instructions I have posted here;

http://www.cnczone.com/forums/madcam...ientation.html

So your lathe has an XYZ setup with a B oriented (in the X axis plane) lathe axis? Are you wanting to mount a rotary C axis on the Y axis and then mount the X axis to the top of the C axis rotary table? So the X axis, angle plate, Zaxis, and spindle all rotate on C?

IF that is what your plans are, I don't think there is a CAM package that will generate movement of the spindle over the part when it isn't oriented purpendicular to the Y axis. You would run into positioning moves where the spindle would be moving toward the center of the C axis (rotational center) but it would be changing in Y position without actually moving the Y axis. The best way to do what you want to do that would be to mount your rotary table (C) over your X axis on a bridge mounted to the XY bearing plate. This way the C axis center is always in line with the XY plane while keeping X movements at a right angle to you Y axis movements and you will still be able to machine anywhere on the surface of the C axis by using fourth axis machining in madCAM.

[Ya-Nvr-No]

Thanks for the reply but I think we have a misunderstanding what I attempting to do. I'll try to explain it another way.

So your lathe has an XYZ setup with a B oriented (in the X axis plane) lathe axis? Are you wanting to mount a rotary C axis on the Y axis and then mount the X axis to the top of the C axis rotary table? So the X axis, angle plate, Zaxis, and spindle all rotate on C?

C axis rotates around the Z spindle axis
B axis rotates around the Y spindle axis
A rotates around X (but I am not using an A axis on the lathe)

I am orientating the lathe spindle (C axis) to a programed angle position from the reference home index (example: say I am drilling a bolt hole pattern around the center of the lathe spindle axis) and then using the X and Y axis with the cross slide table spindle, drill a hole on the face of the part held in the chuck.

But because both the Z axis (the rotary C axis) and the (second XY table) spindle axis are inline, MadCAM throws an error.

So it comes down to why should I not beable to drill a hole in the face of a part, if the rotary axis and spindle axis are inline?

I can do it without using a rotary axis it is just an XYZ move, once the lathe spindle is rotated to the correct angle, I can lock it in position.
0,0,0 All based off center line of part, and part face, held in lathe chuck.
But I have been hand writing code to orient the spindle then move to location and drill the hole.
Just can not figure out how to get MadCAM to do it for me.

Not sure why this seems so confusing, I thought the photo would help.
Both spindles are AC servo drives so they are positional.

On a side note with the second spindle head shown in the photo:
Eventually I'd like to beable to drive the tool on vector lines.
And MadCAM produce both spindle orientation codes to stay on the 3d vector lines. (spindles are not running but used more like for 3d engraving)
As you can tell it is a special application.
C Axis rotates and the XY table travel in Z while the B axis spindle stays orientated and true to the line.
Hope that clears up any confusion.

Thanks again