I’ve been homing my machine, then using the touchplate to find the xyz axes. It’s worked well, except for a few times when I had to change bits in the middle of a cut and things didn’t line up perfectly.
A few days ago, I saw a YT video of a guy that says he only uses the touchplate for the z axis after he homes his machine. I assumed (perhaps incorrectly) this meant he always worked from the machine home and did not use offsets. Then I found the offsets I entered into Mach4 several years ago, removed them and now I’m kind of balled up in my underwear.
There is a place to enter offsets in both Mach4 and Vcarve. Which is better? I think if I used the machine home (without offsets) to set x,y=0 and only used the touchplate for z, I could eliminate the misalignment problem I described above. Am I overthinking this?
I think the answer you want is “yes, only touch off Z when you change tools, but you can still touch of X and Y once per job”.
If you only touch off Z on a tool change, and find that the X,Y don’t line up any more, something else is wrong.
The extra answer is: your machine has multiple “origins” - the machine’s absolute origin (based on the limit sensors) and a handful of “work offsets” selected by G54 through G59.3. Touching off X and Y change the work offsets, so you don’t want to do that in the middle of a job. You could, for example, have four “stations” on your bed, each with their own work offset (i.e. G54 through G57), and run the same job four times with each of the four offsets, and cut four pieces of wood. You may have your work offsets all be zero, which puts your work origin at the machine’s origin.
Your software also has offsets, in that it has some “origin” that is the 0,0,0 point from which other points are measured.
The only important part of all this is that your machine and your software need to agree on where (0,0,0) is.
The center of any bit is in the same exact place, its the axis of your spindle shaft. So you set X, Y, and Z workpiece zeros once in the beginning, and then for any bit after that, you ONLY set Z. This will keep them all referenced to the same place. If you re-do your X and Y zeros for each bit, you will most of the time introduce errors from the touchplate process, either because the touchplate isn’t exactly where it was the previsous time, and the fact that most bits have at least a few thousandths of an inch off from their specified diameter. I have measured some endmills to be 0.007" smaller than spec’d.
The offsets you are mentioning in Vcarve and F360 are for more advanced things like working with jigs or something that changes where the project is with respect to your set zeros. They aren’t really needed for most people.
You just need to make sure you set your X,Y referecnce point in the project (Vcarve or F360) in the same place (like center, or lower left) the same as where you do that for the touchplate.
I use the work offsets in Mach4 almost exclusively. I created a set location on my spoilboard by drilling a series of .25 inch holes parallel with the X and the Y axes. Where those holes meet in the front left corner is my work offset (I set it as G55 in the Offsets tab in Mach4.) Whenever I turn on the machine, I home it, mount the material using steel dowels in those .25 inch holes as alignment guides, apply that G55 offset, remove those steel dowels, load the g-code, set my Z zero with the touch plate, then run the g-code. I don’t need to set X or Y zero, because that location is already known.
I did a multi-color epoxy inlay a year or so ago that involved 15 colors, carved and poured over the course of 6 days. I took the piece off the machine each day and poured the epoxy in the house. The next day, I mounted the piece again, and did the next carve. I used the method I described above, and never set my X Y zero in Mach4 a single time. I used that work offset, and it came out perfect.
I’ve not used the Offset feature in the Job Setup form in Aspire or VCarve Pro, but I know a couple of people who do use it. From talking to them, the same results can be achieved using either method. I use the Work Offset in Mach4, it works for me, so I’ve never taken the time to explore using the offsets in Aspire or VCarve.
I’ve been using your suggestion and it’s working quite well. When I created my spoilboard from 3/4" MDF, I drilled a grid of 3/8" dowel holes 4" apart. I used the dowels to “corner” smaller material near the 0,0 position on my spoilboard, then used the touchplate to find its exact X,Y location. Those coordinates became a new offset in Mach4, which I’ve now used numerous times. I think I’ve finally cleared the brain fog I had around this offset business.
I ran Mach3 on my old CNC router. I used it for about 7 years. I never explored using work or fixture offsets because I thought it was just overcomplicating things. I had a 3-way touch plate to set my X, Y, and Z zero, so no big deal. It was only after I got my Avid 4848 Pro with Mach4 that I decided to investigate work and fixture offsets. I now realize that I had actually been overcomplicating things all along. Having those known locations set up as work offsets really streamlines the work. Now I’d never go back.
