In Carbide Create you get a zero of lower-left, Centre-left, Top-left, and centre. Although my machine zero/home is the back right. Or would it be called the Top-Right. OR am i looking at this backwards an would I really be in the Top-left? Where I have my zero now. Im working -X and -Y which i like much more.HELP
The zero in your Carbide Create (CC) is an arbitrary location. For instance, say you told CC to use “top of stock” (in the Stock Thickness area) and a Toolpath Zero of lower left.
When you’re done with your design, one generates “G code” - instructions that command the machine to create your design. These instruction are performed relative the point you defined.
Now one places the stock that matches that was defined in CC in your machine. Where one places their stock on their machine isn’t really important… where it is the most logical: it can be fixtured so that it cannot move when machined and it is easy for the operator to access it.
Yes, this means that the X0Y0 of your CC part is, most of the time, not aligned with the zero of your machine. In fact, virtually all of the time we’re not interested in the machine zero at all.
How one proceeds from here is somewhat up to how one conceptualizes their CNC machine. I will explain things the way I teach it. Normally, I do all of this over a machine but let’s try this entirely by description.
Say the stock defined in CC was 4" wide, 5" tall, and “0.5” thick. We need a piece of stock a least that big so we obtain our goal. We now have to think about fixturing (e.g. clamps). How does one keep the stock from moving when it is machined?
One common technique is to cut a piece of stock larger than necessary - 5 x 6 (still 0.5" thick) - so one can position the clamps around the sides and have a unobstructed 4x5 area within the fixtures. We can set up the necessary “zeros” anywhere within the boundary that is entirely free of the fixture (no collision will be possible because we’re never there).
Now one needs to align the zero point from CC with the stock in one’s machine. We do this by jogging (moving) the gantry around with the necessary tool in it. One said “top of stock” so one needs to have the tool touch the top of stock and declare this as Z0. Likewise, the corner (“bottom left”) has to be assigned - X0Y0.
Let’s see. Get out a ruler. Find the left corner closest to you. Measure in 1" from the left edge and 1" away from the edge closest to you. Mark that spot. Move the gantry such that the tool is over that spot and just barely touching the stock . Set X0, Y0, and Z0 there.
Review: Now one has Z0 at top of stock and X0Y0 at an acceptable location. The virtual world of CC is now aligned with the physical world of CM. We’re ready to cut.
Where to chose one’s X0Y0Z0 and how to assign it within your machine comes with learning and practice. One creates a “work flow”, a documented procedure one uses to solve things.
The method I presented above is one of several techniques. Over time, and depending on what one uses their machine for, one will develop multiple “set up the zeros” work flows. This is where things like edge finders and laser pointers come in. That’s for another time…
Once one understands things conceptually, all that is necessary is to learn how to achieve it when using Carbide Motion (CM).
There are “jog” (move) and “zero” (set the zero of a job) tabs in CM. With CC, if one uses the larger than necessary method, one can ignore the offset column in the zero tab (that is for a more advanced learning session).
When one’s tool touches the top of stock, go to the zero tab and hit “Zero Z”. When you’ve found the location for X0Y0, go to the zero tab and “Zero X” and “Zero Y”.
Do things make sense now?
Thanks for the overview and a good explanation, I just asked the same question myself.
One thing I would like to point out is that on my machine (shapeoko3) the limit switches are set up top right, looking at the machine from the front. If the toolpath zero was optionally there, it would mean that after I press home there would be less distance to travel to set a new zero point. Currently I would have to traverse most of the X axis if I used the top left toolpath zero. It would simply be more convenient if the top right option was there. Does that make sense?
To get around the problem I just pull the paths down and to the left of the working area / red zero symbol
Once one is comfortable with the zeros - CAD, stock and machine - then one can permute things.
For instance, if ones machine has it’s zero on the right, rather than the left, set the stock zero on the front right… and simply reverse the measurements. Measure from right to left.
Working on as CNC machines as I have, one gets used to have the machine zero all over the place - left or right. The CAM is adjusted accordingly.
Looking at the latest CC I see that it doesn’t offer zeros on the right. That is a pity. Please ask for this.
Until that is offered… jogging the distance is necessary.
In the general case - CC is somewhat of a special case - your CAD zero (where you work your object design from) has to be embedded within your stock. As long as there is sufficient stock to contain the design, the stock/CAM zero can be anywhere easily accessible. The CAD zero now takes a back seat.
The stock/CAM zero can mathematically it can be anywhere on the stock. Not putting at an easily accessible place makes it extremely difficult to ensure proper alignment; a stock corner is the most obvious choice - since this is easy to find.
Stock center is another possibility… but that takes some thinking. That a marker and draw lines from from opposite corners to opposite corners - “X” the stock. The intersection of the lines will be stock center. This technique is not recommended when the zero needs to be very accurate and precise.
The CAM software performs the necessary calculations relative to the stock/CAM zero. One must then align the stock/CAM zero with the job zero on their machine… they need to zero the machine. The job zero doesn’t often align with the machine zero although it can.
As long as the layout of the stock and position of the job zero are in the same relative alignment with the stock/CAM zero, the job is machinable - provided that it fits on the machine and doesn’t collide with any fixturing.
For new users of 3 XXL these explanations are clear as a bell. I am a brand new user 76 yrs young and have been having an extended learning curve on this machine, thank you Mark, I hope to find other “helps” from you in the mass of information held in these forum topics.
I’m glad you found the explanation clear!
The multiple reference points - the zeros (CAD/CAM/Stock/Machine - are often very confusing issues for a new CNC user. Being able to visualize and understand what’s going on takes some doing.
Once one “sees through” this issues - usually by their 3 correctly working job - it becomes “old hat”.
+1 for right-side machine zeros!