Mill the side of a box

[coctavian1979]

Hello.

I'm new to this field when it comes to CAM and Fusion 360 so I have a nub question.

I have a box that sit perfectly on my CNC machine table and on that box I need to mill some holes on one side. I know that the best was to place that box facing up with the side I want to work on  but then it will not fit my CNC machine. I can rotate my spindle 90 degrees so the milling tip points to back of the machine (y+). (Basically I want to plunge the tool on Y axis and move it on Z and X axis instead of the normal way - plunge on Z and move on Y and X).

I've created the model in Fusion 360 but I do not know if I can do this as I do not find the tool orientation that will allow me to basically "swap" Z and Y axis in generated gcode. Is this possible from code and not from changing the wire on the CNC machine to swap Y and Z axis ?

Best regards and thank you for any information.

[LibertyMachine]

No, there isn't a post or software solution for what you are looking to do. This has been requested from time to time, but never really seemed to go anywhere.

Your best bet would be to swap the wires to your motors.

[coctavian1979]

Thank you for your reply.

I was hoping on not to do that but if there is no software solution I will have to go and to that :(.

[djowen40]

I see others have suggested no.

From my point of view the answer is yes it can in theory be done in code but you will require some heavy post processor customization. This is a lot of coding and a lot of testing.

Even then it will be tricky. You wold need to swap the Z and Y axis outputs in you post. You would need to do everything in G0 or G1 moves. Canned Drill cycles will not work as your CNC controller is will go back to using the Z axis.

This could be done but would require some extensive testing. I am not sure if anyone here has done it. I have some ideas on how one might do it but i am just spit balling. I haven't fully thought it through

These two line in the post processor control the output of the Z and Y coordinates

var yOutput = createVariable({prefix:"Y"}, xyzFormat);
var zOutput = createVariable({prefix:"Z"}, xyzFormat);

modifying them to below would effectively swap the Z and Y output as far as your controller is concerned. However this will only work with G0 and G1 type moves anything involving an arc (arc planes G17 etc. will be wrong) or a drill cycle will not work . You might get around this by making a simplified post that linearizes all arcs and expands drill cycles.

Note the prefixes are swapped.

var yOutput = createVariable({prefix:"Z"}, xyzFormat);
var zOutput = createVariable({prefix:"Y"}, xyzFormat);

If you have no idea about post processors then tread with caution.

What CNC controller are you using? 

[coctavian1979]

Thank you for your answer.

This one is more to my liking as I'm a programmer at my core so I'm more into writing software code/modules than tinkering with the hardware as it is more prone to destroying my CNC wires and boards.

My CNC machine is controlled using LinuxCNC trough parallel port. The electronics after parallel port are just a opto-isolated board and motor drivers.

Starting from your suggestion I will start digging into post processor customization and do some learning about G codes.

[djowen40]

Happy to offer guidance. 

If you are familiar with coding then you will find that the post processors are actually quite simple. Post processors are written in java script. You can use you currently working post as a starting point. I haven't put much thought into it but the arcs are definitely going to be the problem. 

Swapping the Z and Y axis is also going to cause the G17, G18 and G19 planes to move/rotate/mirror. Its 11pm here and my brain hurts to much to figure out how things are going to change. I suspect there will be some strange mirroring of arcs.

I would start by just swapping the Z and Y axis and output some simple linear moves (straight line 2D contour with lead-in and lead out turned off) and check that everything move in the right direction. Once you happy with the straight line out and in some simple arcs in a single plane and see what happens.

This will help. 

http://cam.autodesk.com/posts/reference/index.html

You can also use the dumper post from the fusion installed library to see all the raw parameters that re passed out of fusion and into the post processor script. Start by CAMing up some simple straight line moves and then run the dumper. Then add in some arcs etc. you will pretty quickly see how the parameters are built up. 

You could try setting

allowedCircularPlanes = 0; // disable all circular planes

near the start of the post. this will force Fusion to linearise all arcs to straight line moves using the global tolerance (i.e. convert to arch to G1 moves). however again i am not sure how the arc plans will mirror etc. 

quick guidance

function onSection() is called at the start of each new CAM operation

function onRapid(_x, _y, _z) for rapid moves

function onLinear(_x, _y, _z, feed) for feed rate moves

function onCircular(clockwise, cx, cy, cz, x, y, z, feed) for arcs (this will be the tricky one to figure out)

Final thought for the night.

I have no idea how Linux CNC treats canned cycles. However, if you just replace all the cases in function onCyclePoint(x, y, z)  with expandCyclePoint(x, y, z) [or just remove the switch case all together and call expandCyclePoint(x, y, z)] then it will convert the drill cycles to G0, G1, G2 and G3 moves. Assuming you manage to get the arc plans sorted then this will let you use the drill cycles. Caution the expanded code for some cycles e.g. chip breaking requires a lot of moves and may choke you motion controller. 

Brain dump over. Have fun.

[djowen40]

Other thoughts to consider.
1. Your tool length offsets will no longer work as the CNC controller will still apply them to the z axis. (Which is now being used as a y axis) so any change in tool length off-set would correspond to your physical output being translated in the y axis by the tool offset. Essentially you are going to be restricted to one tool per g code output and will need to reset your g54 offset too account for the new tool length on the next tool

2. You work coordinate system in you machine will not be flipped. So y is z and z is y. Jogging could get confusing

If you are into coding you may be able to hack Linuxcnc to reconfigure the pinout in software. E.g. tell the computer to send y moves to the z axis pins on the break out board. I have never played with Linux CNC but there may be a simple config file that defines what pins are assigned to. You could then just swap the config files in and out to swap your axes with having to change wiring

[djowen40 · Accepted solution]

In fact here it is

http://linuxcnc.org/docs/html/config/stepconf.html

No need to crest a new post. Just remap you pins in a new step config. Just make a copy of you current config then swap the z and y pins. You will also need to swap the steps per mm on z and y axis if they have different values

This will fix all the issues without a custom post processor. And will mean the tool off sets etc still work and jogging in z will be jogging in z.

[coctavian1979]

I forgot about StepConf from LinuxCNC package 🙂 That is a good solution. This way I can make 2 configurations, one for normal use and one for swapped Y-Z axis.

Thank you for the valuable info and hints.

In my spare time I will also play with the post files just to see if I can do this directly from fusion 360 😄 ...  Just for fun