Datum offset for one side only in a two-sided project?

[fooyay]

Hello everyone, I'm still learning the ropes and have mostly got the hang of two-sided projects, except for one issue I'm trying to figure out in order to streamline things, because I'm trying to make the process more repeatable so I can churn these items out a bit more quickly and reliably.

I use the asymmetrical dowel method to flip my pieces and it works very well. I have a corner jig set up on my machine (Shapeoko Pro XXL) to position every job I do at the same XY zero. This just saves me from having to reset my zero as often, since most of my projects will work fine from that same starting point.

Is there a way for me to offset just the BOTTOM toolpaths on my two-sided jobs? I run into two issues right now:

1.) If I keep using the same corner jig, real estate is going to get tight in that area when it comes to dowel holes for different projects.
2.) If my stock doesn't perfectly match the dimensions I have in Aspire, when I go to flip it, the jig can interfere, causing me to have to remove the jig and reset it after the job is done, which defeats the purpose of having it.

I've tried using the XY Datum Offset option, but found that it offsets the entire job, and not just the side I'm currently working on. I thought to maybe move my toolpaths to a new sheet, but that messes a bit with the two-sided workflow that I'd like to preserve if possible.

Should I just virtually increase the size of my stock in Aspire? i.e. if my stock is usually 32(x)"x5(y)"x0.75(z)", could I get away with making it 32x10x0.75 in Aspire, so when I go to flip it on the CNC, it thinks it's cutting higher up?

Basically, I'd like to mill the bottom side of my material reliably from the same dowel holes, say, 5" away from my jig, without having to re-zero every time. If I already have my zero set based on my corner jig, I'd like to be able to cut my top side, flip over into the dowel holes out of the way of the jig, and go straight to cutting without having to align and re-zero.

I can take some pics and attach files if needed, if none of this makes sense

[fooyay]

As a quick note:

I increased the Y-size of the stock in Aspire, and for all intents and purposes I think it will accomplish what I'm trying to do. I'll be able to run it through a test cut later today or tomorrow. In the meantime, still curious if there is a way to programatically offset the toolpaths just for the bottom side of the stock?

[adze_cnc]

One thing to remember about the "asymmetrical dowel" method is that you can run the top side at any place on your machine.

Let's pretend we are making 3 different objects (A, B, and C). You could run all your top sides for any combination of your objects whose tops you want to cut in the common top zone. You could then run the bottom sides of a particular A, B, or C in its zone.

An image to help visualize this:
 

[martin54]

I am not sure I understand correctly, you say you are using the asymmetrical dowel method but it sounds like you want to just flip the part over & use the same dowel holes that would be machined for the front of the project if I have read your workflow correctly (probably not knowing me lol).

As adze_cnc has said you can machine the dowel holes for side 2 anywhere you want in the spoilboard. Just jog somewhere clear & set that point as your X Y zero position, then drill the holes to align the part

[fooyay]

Thanks, I understand what you're both saying I think. I guess my question revolves around convenience more than necessity. I'd like to have to re-zero as few times as possible, just to save time. I also want to limit the # of holes I have floating around my spoil board. It doesn't take a ton of time to zero the machine, but over enough cycles it adds up, and also can lead to mistakes if I forget to set a zero at one point.

Basically what I'd like to do is:

1.) Place stock in the corner using my jig. Set my zero once with my bit setter.
2.) Mill the top side
3.) Remove the stock, maintaining my existing zero, and mill the bottom side dowel holes clear of my jig (i.e. 5" higher)
4.) Flip stock and place in the dowel holes, clear of the jig, not have to re-zero, and mill the bottom side

The process after that would then be easily repeatable for future cuts, without ever having to adjust my zero from the corner of my jig or pull out the bit setter again, unless I was working on a different project obviously. As long as I placed my stock in the jig for the top cut, and in the dowels for the bottom cut, I'd only ever need one zero (the jig).

But, if I mill the top, and then I jog manually to get clear of the jig, and set my XY zero for the bottom, then I'll have to reset it again back to the corner of the jig if I want to do another TOP side. And if I later want to re-use these same dowel holes for the bottom, I'm not totally clear on how to return to them without having to put my stock in the dowel holes, and then use my Bit Setter/probe to manually re-zero. I don't want to have to drill new dowel holes every time I need to cut a bottom, either.

example:

1.) use bit setter to zero @ my jig, making note of machine coordinates
2.) Mill the top
3.) Jog elsewhere, make note of coordinates, set zero, drill dowels, flip stock, mill bottom
4.) Manually return to coords from step 1, reset zero
5.) Mill another top
6.) Manually return to coords from step 3, set zero, mill bottom

Hopefully I'm explaining that well enough. You could call it laziness, but extra steps really do add up, so I'd like to eliminate them where possible, and also keep my process as repeatable as possible. Of course I see some of the issues with this as well: if my jig ever moves, all my dowel positioning will be messed up as well, in which case I'd have to start it all over. It's also somewhat limiting to set in stone that my dowel holes will always be 5" higher than my origin.

I think my solution of making the software think the stock is bigger than it is will solve the problem. But maybe a better solution is to see if I can figure out how to track my zero coordinates for my jig & for my dowels, and reliably return to them with Carbide Motion. I don't know GCode and I'd prefer to deal with GUI's than with code, but maybe that's the way to go.

Unless I totally misread what you guys both said. In which case, if you can set me straight, please do! But it does sound like there's not really an offset feature like I'm looking for in Aspire, anyway.

[fooyay]

To close this out:

Virtually up-sizing the stock by 5" in Aspire worked just fine. It's an easy enough solution so that no matter where I mill the top (i.e. if my jig moves for some reason), the bottom dowels/side will always mill 5" away, out of the way of the jig.

But I also finally learned some basic GCode to just jog the machine to existing coords, which I didn't know I could do as easily in my controller app. For future projects, I think I'll just keep a spreadsheet of machine coords for various dowel positions, and I think that will work as far as repeatability goes as well.

Thanks for the suggestions/breakdown all!

[martin54]

I can think of 2 ways that would work, first use sheets & make your second sheet bigger, copy the bottom to sheet 2 & then move it your 5 inches in x or y. Everything would zero off your original X Y zero position but the bottom would be placed & machined the 5 inches offset that you wanted.

The other way would be to learn how to use work offsets/fixture offsets within your CNC control software, these are G54 - G59 settings

If you use the same size material a lot for these projects then save your file as a template & just use the same dowel holes over & over again.

[BrooksM]

Hi fooyay,

If I understand what you want to do, you might find Mark Lindsay's interesting.



Good Luck,
Brooks

[rscrawford]

Rather than change the X0Y0 in Aspire for the second side, simply change it on your machine.

Many controllers allow you to save positions on your machine. I have many different 'home' positions saved on my machine in WinCNC, and am able to accurately use any of those positions for years when I do two sided projects.

The beauty of index holes to flip your project, is that you can cut the first side anywhere you want, then set a new local X0Y0, cut the index holes in your spoilboard, and use that new spot to cut your second side.

[SteveNelson46]

Rather than change the X0Y0 in Aspire for the second side, simply change it on your machine.

Many controllers allow you to save positions on your machine. I have many different 'home' positions saved on my machine in WinCNC, and am able to accurately use any of those positions for years when I do two sided projects.

The beauty of index holes to flip your project, is that you can cut the first side anywhere you want, then set a new local X0Y0, cut the index holes in your spoilboard, and use that new spot to cut your second side.

I use this procedure almost every time I cut a two-sided project. It works great

[fooyay]

All, thanks!

Yeah, I solved it basically using all your suggestions. I think just writing down the coords and returning to them manually is actually a more elegant/versatile solution than trying to do it programatically in the cut file itself... it's really just one command to get back to that spot, anyway.

So I went to my JIG ZERO, wrote down those machine coords and put them in a spreadsheet. Cut the top side, then jogged a few inches away clear of my jig, wrote down the new DOWEL ZERO, cut my dowels, flipped the stock and milled the bottom side.

Then to do another one, I just returned to my JIG ZERO through Carbide Motion MDI interface, reset my zero, rinse and repeat.

Carbide Motion doesn't allow storage of different zeroes, so I have to return to them manually, but having them in a spreadsheet makes that easy enough.