[Stewyau]

I've just got a new 5 axis mill and am working through madcam 5 (great program) the toolpathing is pretty straightforward (after much practice)
but the problem I'm having is that the simulation looks fine top planer surface followed by a front planer surface, but when I run the toolpath in the mill, the z height of the top down is fine, it stays above the 4 jaw chuck but when it flips to do the front face the cutter goes back to x and y zero which is at the base of the chuck, I'm thinking there's something that i need to add to the post processor (mach3 5th axis) !!!

[Dan B]

Does your controller support TCPM? (Also referred to as RTCP). This feature allows the tooltip to stay in relation to the part 0. Without it, you are going to have to factor in the machine kinematics for your rotations. I would think that you must have some version of that.

See if you can use M128 (TCPM on) and M129 (TCPM off). Also see if your controller supports M126 (rotates to the next angle with the least movement. For example, if you need to rotate 359°, M126 will cause a -1° move, not a +359° move).

Start there. Once you understand the available features, it should be easier to customize a useable post.

(Unless I totally misunderstood the problem, if so, please let me know).

Dan

[Stewyau]

I can't find anything about mach3 have the TCPM capability, i'm guessing that it doesn't
I've attached a link to a small video that probably explains whats going on better,

Stewy

https://www.dropbox.com/s/ymiznv534v...001_214128.mp4

[Dan B]

Okay, I see I did misunderstand. I thought the initial path was good, and it was losing it's orientation when rotating 90°. I see it's the other way around. Can you post the model with your toolpaths? I'm assuming you've picked up the center of your chuck as X0Y0? Where is Z0?

Dan

[Stewyau]

Dan
the origin is at 0,0,0
the mill is fixtured/set at 0,0,0
the model has z raised up in rhino to clear the fixtures
Ive included the test piece and the toopath for you

stewy

[Stewyau]

sorry Dan
the fixture is set x0,y20,z0 so the cutter will clear the chuck when doing a cut parallel to Y, but i can change all this, i've set it this way due to the machine doing a home and probe after your first fixture set up, I have to have the cutter protruding out of the tool holder only 5mm for it to touch off on the probe (first time only) , i did have it set up this way but the problem is still the same, but with 0,0,0 set up the top down is good and the flip is out

Stewy

[Dan B]

I guess I'm still at a loss as to how your machine/controller handles the machine kinematics without TCPM functionality. How does the location X,Y,Z get transformed to the new rotation?

Here is a discussion on this subject for the mach3 controller:

5 axis kinematics and coordinate transformation

Follow this link too:

cnc4free.org homepage

Sorry, without familiarity with that controller I can only be of limited help. We have Heidenhain controllers on all of our 5-axis machines, so we are able to use a variety of methods to transform the coordinates to the new plane (M128, PLANE_SPACIAL or CYCLE 19).

Dan

[Stewyau]

Talking to a guy about it who does the support for the mill in the states, what they do is to set up another fixture offset,
so the fixture offset i have now g54 will do the 3 axis flips , then itell the machine to go g55 a new fixture and do the top down (sounds easy doesn't it......)
I'm pretty sure deskproto can do it with there multiaxis version as you are able to enter your own code when your setting up your toolpaths, then you just post it from deskproto,
I guess you would know if something like that is possible with madcam?

Stewy

[Dan B]

Yes, you can do fixture offsets in the madCAM post-processor. You need to add a section to your post like this:

*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;G54
*END_SECTION*

After adding this section, you need to add the variable where you want the offset to appear. Here is one that I use:

*FIRST_MOVE*
N"lnbr" G00"x""y""fixture_offset"S"speed"M3
N"lnbr" M300Q4
N"lnbr" G5.1Q1
N"lnbr" G43D"toolnr"H"toolnr""zhome""coolant_on"
N"lnbr" G00"zhome"
*END_SECTION*

Now when you post, you will get a field in the post-processor box that will allow you to pick the offset you want to use:

Attachment 203112

Dan

[Stewyau]

thanks Dan

stewy