Official Luthiers Forum!

How does a CNC find the starting point? This seems like such a basic question but it also seems to have broad implications for how time consuming it is to do small runs or one-off items like many small shop builders do.

Do some of you have different table tops that just plug in with hold-downs or indexing already incorporated? One table top with lots of indexing?

Thanks.

_________________
http://www.chassonguitars.com

That depends, If the CNC has home switches, then homing the device allows a constant start point for all axis to reference from machine coordinates to set work coordinates. Now if no switches exist, then the operator will most likely start with a work coordinate somewhere on the table as a reference and zero the machine. You must assume that when the toolpaths are created that the operator knows where X0,Y0,Z0 is designated by the code for the particular operation. Meaning X0,Y0 is located at the center or left bottom corner, right top corner and so on in reference to the workpiece. As well as Z0 is the top or bottom of the workpiece.

I hope that helps?

MK

_________________
I'm outside looking in, just farther from the window than most.

I was in the same boat as you just a few months ago and here's a couple threads I started on similar topics:

viewtopic.php?f=10106&t=32852

viewtopic.php?f=10106&t=32850

I use hall effect home switches which are very repeatable. What I ended up doing for my indexing is bolt down a semi-permanent fence to the table with a long X-side and a stubby little y-side. Originally, the fence was a little proud of what I need and then I used the machine itself to cut the face of the fence at exactly X0 and Y0. Actually It's probably off by .001" because my endmills and a tad smaller than their size (e.g. my .250" endmill is spec'd at .250" +0 - .002)

What I do is either mount my workpiece right against the fence or, I mount a vacuum jig that's butted up against the fence that has locating pins in it which I use as my origin. I then use an offset (G54~G59.X) to so that the machine knows where it is.

I've found that this setup is extremely repeatable - like better than .001". The plus is that if I need to remove my table for maintenance or adjust my home switches, re-tram my spindle or whatever, I simply make a new fence out of MDF and re-cut it with the machine.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I'll assume the question was more basic.

Let's assume you have a piece of wood in the jaws of a vice that's mounted to your table. You can mount a probe into the spindle. Then you jog the table or gantry to make that probe touch off the right side of the block. The machine knows where it is...so you push a button to tell it to remember that position....that's the X origin. Next you move the probe to the far side of the block and do the same thing...establishing the Y origin. Lastly, you put a cutting tool into the spindle and bring it down to touch the top surface of the wood...establishing the Z origin....but only for that tool. All subsequent tools will have their own unique Z heights to program...since they are each mounted into the holdler at different lengths.

Now...if your cad model is drawn within a block that represents that chunk of wood out at the machine...and the origin is in the upper, back, right corner....you are ready to start programming your tool paths. If your model isn't drawn in the right position...a good cam program should allow you to draw a box around your part (representing the wood blank) and move it or turn it to get it into the correct position.

When the machine knows where that corner of the wood is....and the software references that same corner....push the green button.

When setting up a job I often use a work stop so that I can simply loosen the vice, remove the part, put in a new block that slides over to the stop, then tighten the vice. With vacuum fixtures a pin, a slot, or an edge can be cut into the part on a previous operation to register the part onto the tool prior to turning on the vacuum. When cutting from a raw block it's not necessary to be spot on accurate when placing the stock in the jaws or onto a vacuum fixture because you're probably cutting all the surfaces away anyway. But when you are doing second and third operations on a part you may need to make a set of custom jaws to hold the part according to its specific shape. That results in the part being placed into perfect postion every time. In this case I'd program the machine to know where the back, right corner of the jaws is...and then draw the jaws in my model.

Most of the time, when drawing a part, I also draw the tooling fixture that's going to hold it as part of that model. Then, when I import the whole thing into Mastercam, I simply move the whole business so that corner of the tooling fixture is the origin.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic

Hello,

I think that you will find this video quite helpful:

http://www.youtube.com/watch?v=IWglgxdFpVE

Let us know if you have any more questions....

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

I just do it visually. I mount the piece offset from the edges. I jog the router to the appropriate zero point of the piece I am machining. Then move the X axis to the other side of the blank to make sure the blank is square to the table. Then back to the 0,0,0 point. In Mach3, I zero all the axiz and away we go. If I have to be really precise I put a pointed bit in to determine X and Y zero, the put the real bit in to determine the top of the blank.

Thanks all. That's exactly the info I was looking for.

_________________
http://www.chassonguitars.com

I do all of my designing in Rhino with X-zero and Y-zero falling in the center of the design. Makes it easier for me to machine around center laminates in neck blanks, centers of bookmatched pieces etc. I use indexing pins and vacuum on all of my jigs. The way that I zero the machine is that each of my jigs has a 1/4" hole drilled at 0,0--when I make my fixtures, I've included this hole in the original CAD design so that everything will fall in the right place. I take a piece of 1/4" inch drill rod and chuck it up in my spindle, then jog the spindle until the drill rod will drop straight into the hole in the jig. Actually, I usually do this with the emergency stop kicked in on the controller, and dial the position in manually with handwheels on my steppers, then un-do the E Stop. At that point I set machine 0 for X and Y. I never had as much luck setting 0,0 on a corner because of slight differences in size of my material. Using the absolute center instead makes the size of the material less relevant, and my centerlines always fall in the right place regardless of any asymmetry that might be there in the material to be machined.

Probably not the most elegant way of doing things, but it works for me.

Dave

Dave,

Add homing switches to your setup. You'll love it and save a bunch of time!

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Thanks Andy.

Yeah that's what George says too! But it only takes me maybe 20 or 30 seconds tops to zero x and y, and I can put my fixture anywhere on the table I want to this way--no indexing of the fixture to the table is needed. Just make sure it is square to the axes, and it's good to go. I can also position multiple fixtures on the table concurrently without having to figure out offsets if it's a one-time combination (I do use offsets on my often repeated operations, with multiple fixtures built together on one master fixture). I am installing limit switches on the new machine though since zeroing out the way I do makes soft limits not so useful.

If I used a corner as home, I'd definitely add homing switches but using the center like I do, I like the flexibility. Having handwheels on my motors for easy manual positioning is the key. With my older machine, I may well add homing switches since the table is really too short to use multiple fixtures at once for the stuff I'm doing, so 0,0 is almost always in the same place...

Dave

It sounds like you have your process down but I just wanted to re-iterate one point that maybe wasn't clear - I use the corner as a reference to the vacuum fixture. The vac fixture then has a pin that I use for the origin for the program using an offset so, I still get to use the center of the piece as the origin if I like.

I do think that homing switches do have the advantage of setting up repeatable machine coordinates as well. Without true machine coordinates, my tool change wouldn't work because the controller would have no idea where the fixed plate is. There's also the issue with the soft limits as you mentioned. If something goes wrong and I have to hit the e-stop, all I need to do is re-home the machine and run from here to pick up where I left off.

Thing is - if you install limit switches, you've installed home switches.

p.s. I do not own any stock in any home switch conglomerates or anything like that.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I second what Dave said. I have switches at the corners, but those are shut-off switches so I don't blow out my screws if I do something stupid. I like 0,0 to be the seam on a guitar body, so having the corner be zero doesn't work unless you always use precisely the same size blank.

I think I'm still not getting my point across - there's no reason you can't do both.

I've attached a picture of my fretboard fixture mounted to my machine. You can see that it's butted up against my fence so that the fixture 0,0 was the corner. This was the origin I used to machine the fixture itself.

You can also see the centerline machined into the fixture and the "fretboard origin" which is the hole in the upper corner of the jig (the other hole a bit lower was a screwup - the machine stalled and missed a few million steps when trying to drill the hole at the other end of the fixture - fixed by oiling the ballscrew). The fretboard origin is at a known offset to the machine origin.

When I cut a fretboard, first thing I do is find the center of the fretboard at both ends. A lot of fretboards aren't square when you get them, they're often tapered. I then line that up by eye with the centerline on the fixture. I then run a little program the drills two holes in the fretboard for locating dowels.

I then insert two dowels into the FB and flip it over. Using the offset to the FB origin, I then machine the visible side of the FB.

This way, I have my machine coordinates using my home switches and the ability to index the centerline of the FB for machining.

As I mentioned before, indexing the fixture to the fence has proven very repeatable. When I re-mount the fixture, I chuck up a 1/4" broken endmill upside down into the spindle, activate my FB offset and go to 0,0. So far, it's slipped right into the hole perfectly every time.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Andy,

Looks like a good setup you have, and I can see your points. The main thing I can see from your approach is that you are seeing the machine table with material on it when you start out working a design in CAD while I'm just seeing a piece of raw material. Your approach makes more sense really, and I might be able to eventually force my thinking along the same line.

As it is, I guess I'm showing my age and background as well as the difficulty in teaching old dogs new tricks! All of my design work in the past was focused exclusively around a part (and done on paper with drafting tools no less), and then moved over to a manual machine. Two separate processes, and with CNC two separate processes for no real reason. As it is, with my production jigs pretty well built and with the expectation of having multiple fixtures on the table at any given time (not necessarily directly related fixtures though), I'm still not sure it would make sense for me to change the way my origins are set. I have some new projects coming along where I'll give your method a try though--it is a much more integrated approach than mine has been.

Dave

Is another way of saying that that Andy's drawings all have the table (and zeroed fence) included and yours are just the part?

Big picture, conceptual stuff like this is really helpful to a beginner.

My original thought was to have a few dedicated auxiliary tables with indexing for each part. Maybe one for multiple fretboards, one for headplates, one for necks, etc. Each table indexes into the machine table. Would that make sense?

Seems like half the point of this is being able to set it up and let it run while you are doing other things. If I have to stand around and plug in parts every ten minutes, I might as well machine them myself.

_________________
http://www.chassonguitars.com

Not to answer for Andy--but my understanding of his approach is that he does his CAD drawings with the 0,0 origin in the same corner as his home position on the machine and measures everything relative to that. He does a centerline for his fingerboards in the CAD design so that he has something to sync his workpiece to, and all of the indexing pins to keep it consistent--all relative to his 0,0 that matches his machine. What I've done is to design something without regard to the machine itself, and habit has me setting my 0,0 point to the center of the work. It doesn't take the machine into account at all--I zero the machine to the jig, wherever the jig happens to sit on the table.

From my point of view, each approach has pros and cons. I think that Andy's more integrated method is a more logical solution all in all than mine. But mine has the advantage of being able to put a bunch of different fixtures on the table wherever I can fit them and set the 0,0 where ever I need to. With the handwheels and index hole for zeroing the machine out, it's quick and easy, but not as logical or as automated as Andy's approach.

One fixture that I use a lot makes necks, fingerboards and peghead overlays. Three separate vacuum jigs on one secondary table. It fits in index holes on my main table. I zero the machine to the center of the middle jig on the table. This becomes offset G54. I have also set up G55 and G56 for the other two jigs on this fixture. This same setup would work well (probably better) using Andy's approach, but I would assume he would use G55, G56 and G57 or else he would have made the entire fixture as one big CAD drawing with the whole thing in G54.

I leave this fixture on my machine a lot, since I can do so much of a banjo using just this one fixture. But I also have other fixtures that I use for other things--some banjo related, some not. I'm basically lazy and don't want to take my main fixture off just to do a quick job on something else, so I just find an open place on my table, and put the other jig wherever it will fit. I re-zero the machine to the zero point on this jig, use G54 and I'm good to go no matter where on the table it's sitting. Of course, if I zeroed like Andy does, I could still re-zero manually for the extra jig.

Guess it's all a matter of habit. I like Andy's approach, and I suspect it is probably the more common way of doing things out in CNC land. It's also a lot easier to find a CAM solution that will work with it--pretty much any CAM out there will let you set up a corner origin, but finding one that will inherit the non-corner origins I'm using from a CAD drawing is not as easy. MadCAM does a great job of taking whatever origin I use in Rhino, but most of the other CAMs I tried weren't so forgiving. Starting from scratch, I'd use Andy's method. As it is though, I've got a lot of CAD designs, fixtures, etc. that I don't want to re-engineer. Going forward, I might well change my ways, but for the stuff I'm already doing, I have too much time invested to re do it now, especially since it's not a big deal to zero the machine manually anyway.

Even though I've done mechanical design work for years and I've worked with servo systems for years, I'm a newbie in the CNC world. Trial and error is my game, and sometimes I get it right and sometimes I smack my head and say, "Dang why didn't I think of that!"

Of course, on the other hand I might have completely misunderstood what Andy's doing! The work he's turning out is sure looking good whatever it is he's doing, and that is after all the bottom line!

Dave

Kent,
My K2 has home switches and mach3 has a button that you click on to send the router to that spot in the rear left corner of the table. I then manually move the cutter to my zero position which is on the centerline at the lowest point of most parts. I use a pointed dremel tool to set it there in the X and Y. A click on the software will zero those locations out. Mach also has a tool height setting button for Z which can be used with a metal block to set the Z.

I'd love to have that CFox inspired dead head sander in your shop. I bet it is much faster than cncing a neck.....

Charles is still the best jig designer I've ever met. Clever, simple, "Why didn't I think of that" solutions that are just great. That dead head sander for making necks is brilliant--wish it would work on asymmetrical necks like five string banjos have!

I got my start in guitar making back in the 70s up at Earthworks with Charles Fox and George Morris. I still marvel at how much I learned from those guys...

Dave

The deadhead sander works very well once you get the belt tracking. If it were a dedicated machine, that wouldn't be a problem but I don't have the room. Once set up, I can do 12 necks an hour but there's still the heel to do. And I'm not trying for perfection. I just use one profile and leave it a bit oversized so I can customize by hand if a client requests it.

It would be nice to be able to cnc the heel and sand the neck. The heel needs precision because it goes in a pocket for my adjustable neck.

_________________
http://www.chassonguitars.com

I use SolidWorks to design my stuff and the assembly feature makes this easy and possible but it's not absolutely required - I'll get to that in a second.

What I do is design the part first. Next, I create an assembly and make the fixture for holding the part and start making holes for locating pins. Where the pins go depends on the part.

I then create G-code for the fixture and the part. The fixture is always butted against the fence so its origin is always the lower left corner. The part is aligned to locating pins so I pick on of those as the part's origin and figure out the offset from the fence which is located at machine 0,0.

I haven't fully automated my offsets but but ultimately, my plan is to have one or several G59.x offsets for each jig, hard code that into my controller, write it in sharpie on the jig and code it into my CAM software.

You don't need CAD software that supports assemblies to do this though - you can do it with any CAD software so long as you keep track of what's going. You can manually transfer the orientation of locating pins from one drawing to another very easily so long as you plan ahead.

What you do need though is some repeatable zero on the machine. After looking into it, the fence in my picture above was the simplest to implement and the simplest to re-implement if you have to make any adjustments to the machine. I had investigated drilling holes in my machine to allow the indexing of work tables just like you write but, if you make any small change to the machine (e.g. tram your spindle), you have to adjust everything to match the new spindle zero. By making a simple fence that I can re-cut after making an adjustment I avoid all that hassle. I even made my fence so that I should be able to re-cut it 2 or 3 more times before I need to make a new one.

p.s. attached is one of the more complicated fixtures I've made. I could make that all go away with a 4th axis but judging from the dirty look SWMBO gave me when I brought it up, I should probably wait a bit! All the extra sketches you see are containment and indexing things for my CAM software.

p.p.s. Do keep in mind that I'm also a noob to all this stuff so there are almost certainly better ways out there on how to do this. I do tend to do a lot of investigation before committing a bunch of time to trying a particular method.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Oddly enough, on banjo necks the heel to body joint is the one major machining operation that I don't do on the CNC. It's still easier for me to do those precisely on an oscillating drum sander and a jig (OK, I made the jig with CNC...). A banjo neck joint is a butt joint but with an arc to match the rim and all at the angle of the neck set. My necks are adjustable too, but still easier to do the old way. Funny how different the tricks of the trade are with different kinds of stringed instruments!

Dave

I'm afraid that I'm a "jump into it and see what worked and what didn't" kind of guy. I spend some time researching how others are doing things, but I have to admit that probably the biggest kick I get out of the whole woodworking/machining/building thing is going solo and figuring out how to do something while working in a vacuum. Not the most practical way of doing things, but I've always been moved more by the journey than the destination. "Doing it my way," practical or not, is where I get the most satisfaction.

There's almost always a better way, and I love to see how other people approach and solve a problem, but to me it's the process of discovery (that really only happens by trial and error) that keeps me going. Probably also what deservedly attracts the most snickers! Like the old joke--"Who do you expect to please with THAT??" "ME!"

Dave

LOVE what you are doing with Solidworks! Keep up the good work...



..oh, and go get a PC!

_________________
-CyborgCNC
http://www.cncguitar.com
https://www.facebook.com/CncGuitar

Thanks but, I think I'll pass on the PC - my computer life gets simpler and simpler the more I avoid windows products

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

So I guess I will throw my .02 cents in on home switches. Whether someone uses 0,0 at center or from a corner is not relevant to the use of home switches. They are used as a method to obtain repeatable machine coordinates. By doing this any fixture based somewhere on the machine table can now be repeatable. No matter what the 0,0 work coordinates used.

So if I have a part that uses 0,0 center. Say a 5"x5" part. let's assume I move from machine coordinates to X10,Y10 and zero at these coordinates for my work piece. Now I have a fixture point for my 0,0 center. If I make a locator hole from that center to say X-3,Y0 and another at X3,Y0 in the table, I also take my fixture and make the same holes in the bottom for locator pins. I now have the repeatability with that fixture.

So when the time comes to use it again, The fixture has the corresponding locators. all I must do is either use a G55 or similar call to the X10Y10 location and place the fixture. which is now zeroed for X,Y. Or one could use MDI and go to the X10,Y10 and zero X and Y there. Either way, the use of home switches will ultimately simplify the machining operation. someone mentioned they had limit switches and no home switches. These can also be used a home switches at the same time. They not only protect your machine but serve the purpose of homing as well.

So, I know what I have said is just a repeat of others in maybe different way of explanation?

Mike

_________________
I'm outside looking in, just farther from the window than most.