Help with specifying to Rhino where my CNC's table is

[btsioles]

Hello,

This is my first time posting, so I apologize if my question is really dumb. I'm pretty new to all of this.

A bit of background (again, sorry if it's overkill, but I'd like to provide as much info that seems relevant). I have designed and built a small 3 axis CNC router for the purpose of learning how all of this stuff works. I am using mach 3, and rhinocad/cam. My machine is setup as follows in Mach 3:

Z-axis - 3 inches of travel
X-axis - 10 inches of travel
Y-axis - 13 inches of travel

If you're looking at the machine, Z is attached to Y making up the gantry. That entire assembly is mounted to guides/screw at the base of the machine giving me axis X. The stepper on the Y-axis is oriented on the right of the machine. The X motor is behind the machine, and Z of course is on top. Basically like what you'd see on a K2cnc machine.

Also, I'm using the mechatronics 3 axis controller board. I have limit switches on the motor end of each axis that are connected to the controller which stop movement all together. Mach 3 doesn't know when a limit is tripped since the controller doesn't talk to Mach. I have defined soft limits in Mach at the opposite end of each axis.

Here is what I do to "home" the machine. I jog each axis to the limit switches until they trip. I then hand rotate each axis until the limit switches release. I then set each axis to zero in Mach 3. So, I guess "home" is at that location since that is for the most part a very repeatable spot to bring the machine to. Also, when I jog in Mach away from each stepper motor, the position value increases. I set it up that way since that seems intuitive to me in relation to where my "home" is. Perhaps setting it up that way is "wrong"? The reason I have it setup that way is because I figured, "what if I have a big part that I want to cut, and making "home" somewhere else (like a point at the machine's cutting table surface), would not be possible due to the part taking up a large Z value. For example, What if my stock box is 2.5 inches tall, and takes up most of the cutting surface? How am I to use a reference point at the table's surface for 0,0,0? Also, what if I'm using multiple bits on a piece, and what was the top of the stock box is no longer there for the second bit?

My main question is, if I want "home" to be where I currently have it, how do I tell rhinocam that is where home is, and the bottom of the part to be cut will be resting down on the machine's table surface, and Z should travel down toward the table surface to the box stock?

If the "home" position is repeatable, and rhinocam knows the length of my bit, and if it knew where the table surface was, and that the stock was sitting on that table, shouldn't it be able to process the part without me needing to jog and touch a certain point on the stock or part or table?

I'd like to just put the stock on the table, load my bit, and hit go, and have the machine process from the top down toward the table.

I've been googling for a while to see if anybody is doing it this way, and I'm just not sure.

I'd appreciate any suggestions on what I'm missing. Perhaps what I think should be possible isn't?

Again, I apologize if my questions are so dumb I'm out of line posting...

Thanks,
Bobby

UPDATE - It looks like my Z going upward away from the table should increase the value, and down toward the table should reduce the value. So, I used the "reverse" option in Mach 3 on my Z axis to make it work that way.

I went through the 1st part of the "gasket" tutorial in rhinocam. I posted the operation. I loaded it in mach 3. In order to cut the part properly, I have to jog the tip of the cutter to the corner of the stock box that was defined as 0,0,0 in rhinocam. That's fine, but now what about my soft limits in mach 3? If zero is defined as a corner of the stock box, your soft limits are basically pointless, right? The soft limits are in relation to zero, and if zero isn't positioned at one extreme of each axis, then the limits on the opposite ends of each axis won't work. What am I missing? Do I have to move my part in rhinocam well below the MCS/WCS defined so that it simulates the part sitting down further on the table of my machine?

I guess I just have to make my machine mirror the default orientation of the axis in rhino...

Sorry for the dumb questions.

[mredburn]

Your trying to combine two seperate things into one. You tell Rhino cam where you want the part to be located in your part box or cylinder. You tell it where you want the stock box to be located by assigning the xz points, it then tells Mach where the part and the stock are to be located in relationship to each other. You set up a jig to hold your stock and zero your z, x, y axis, run your cuts. then repeat.

CHoose your stock profile .. box stock. part box stock etc (yellow box under the set up tab)
pick "set to box stock" option in the locate world coordinate system tab

Choose from the zero face buttons then the zero position buttons this will tell R/C where to Tell Mach you want to locate your work at.

Under the RHinocam 2.0 tab at the top of the page choose "getting Started" on the evaluation page that pops up choose "GSG"

Read it.

Mike

[mredburn]

Second you need to read and watch the tutorials on Mach again. YOU dont need to home your machine to the switches for it to cut your program. It does help to tell mach where things are at but it will run the programs without it. You just have to set up your part and cuts so it doesnt run into the limits of the table.
If you make tool changes when cutting a part you will have to re Zero each tool at the time you change the tool unless you have a preset tool depth for each tool. LIke a collet on each tool to preset the depth the same. Some people use a zero touch off tool. You can set up a place on your work stock that wont be cut and re zero all your tools off that point. I know it can be very confusing your trying to learn 3 differnt programs at once. CAD,CAM, MAch. IN RHinocam you will need tomake sure you asign each tool a different tool number. that way Mach knows to stop and indicate a tool change by you before proceeding. IF you dont Mach will continue to run all cuts with the same tool. Been there.. I have had my number 1 tool an endmill run its cuts and then needed to drill a couple of pilot holes . THe pilot drill was also the number one. Mach went through the 1/4 endmill cuts and then proceded to drill my pilot holesw with the 1/4 end mill.

Mike

[mredburn]

Third. I have cut larger parts on my Taig mill than the work table i use. You set up your work the same as always. then you can either make indexing holes and use them with pegs to move your work. You can scribe a line with a very small bit and move the part. My Taig has a 5.5 by 11.5 cutting work area. I have milled 27 in long bars by milling the first ll inches, Starting the cuts with X zero at the left edge of the work table, making a mark at 10 inches with a very sharp small V bit or .1mm cutter and then after I run my first cuts I slide the bar to the left and by using a 10x loup I recenter the bit on the line I scribed and Tell Mach this is where 10 inches is now. (where the zero was to start with.) Then I make the nest cuts and scribe another line with the v bit at 10 inches to the right, ( the machine thinks I'm at 20 inches) move it again and finish my cuts.

I have cut 10 inch diameter wooden clock gears for my father by putting 1/4inch holes in the design that i drill through the part and into a waste piece below it. I then use 1/4 steel dowels to keep the parts in place, make my first cuts rotate the piece 180 degrees and make the final cuts.

Mike