Techniques for two-sided builds

[jeremiah.peschka]

Long time lurker, first time caller...

I've been learning CNC to build guitars, but one thing that's been a frustration is getting two-sided builds to come out with virtually no misalignment.

Historically, I've had a few missteps that have resulted in significant misalignment. Today's process is:

• Placing the blank on the CNC.
• Drilling two holes along the center line (ish)
• Placing the blank on a pair of fixturing pins in a fixture plate from Saunders Machine Works.
• Securing the blank so it doesn't wander.
• Setting zero based on the top and center of the material. I'm finding the center by going corner to corner.

Unfortunately, there's still 1/8" - 1/16" misalignment between the top and bottom of the body. It's not awful and can be taken off with a table router, but I'm wondering:

How do y'all ensure that you can reliably flip a guitar on the CNC so you can do two-sided work?

[mistermikev]

On 9/5/2023 at 8:46 AM, jeremiah.peschka said:

Long time lurker, first time caller...

I've been learning CNC to build guitars, but one thing that's been a frustration is getting two-sided builds to come out with virtually no misalignment.

Historically, I've had a few missteps that have resulted in significant misalignment. Today's process is:

• Placing the blank on the CNC.
• Drilling two holes along the center line (ish)
• Placing the blank on a pair of fixturing pins in a fixture plate from Saunders Machine Works.
• Securing the blank so it doesn't wander.
• Setting zero based on the top and center of the material. I'm finding the center by going corner to corner.

Unfortunately, there's still 1/8" - 1/16" misalignment between the top and bottom of the body. It's not awful and can be taken off with a table router, but I'm wondering:

How do y'all ensure that you can reliably flip a guitar on the CNC so you can do two-sided work?

well... I wouldn't say that I'm an expert on this subject... as I've had varying degrees of success... but I have learned a lot lately. 

Just using my eyes and a center line and going to the back, align, then going to the front and align... I was able to get within 3/16. 

I've since started using 4 index pins... but I was drilling index holes and then flattening my stock after... and this got me to 1/8" accuracy.  This was all w/o using limit switches. 

Now I've setup my limit switches and a light has gone on... used to always worry about finding my ctr after pwr outtage before... no longer an issue.  I have yet to cut another two sided body/neck since I've set this all up but I'm pretty confident things will have improved.  my index holes are now standardized and drilled into my spoilboard -cut after homing my machine and then setting up on offset on the offsets page.  I've have verified that my bit will go back to exact ctr every time now.  so even if I bang it off the walls... I can home the machine, then select my offset... and it will go back to the EXACT center I set.  

So many folks tried to tell me to do this... I wish I had listened sooner.

so much can go wrong that you don't think about when building.  if you run into the walls... you've changed your center... a machine can loose a step here or there and it will look some precision on the center,  backlash in your machine can change your center.  altho in theory none of this should happen...  all of this is corrected by using limit switches, and setting up an offset because the machine will find your center again reliably.  

hope something there helps.

[jeremiah.peschka]

Quote

hope something there helps.

Yes! I had to read your post a time or two, but it clicked!

I'm using a Shapeoko with limit switches and Carbide Motion has 9 pre-designated homing positions. Doesn't matter if they're an inch or a foot away from zero, it's a known reference point which then makes everything else easier.

Thank you!

[curtisa]

Limit switches will only provide a relative reference for your machine for all subsequent operations. There are a lot of other ways for a front/back operation to fall out of alignment that limit switches alone will not correct:

• Backlash on axes (if any) cannot be compensated using limit switches and may result in the tool being further away from the commanded position than the CNC software thinks it is, which will translate to misalignment from front to back when the workpiece is flipped over.
• If the north-south travel (Y) is not perfectly perpendicular to the east-west (X) travel you'll see misalignment. Same problem will exist if the Z-axis is not perfectly perpendicular to the CNC bed.
• Rigidity of the CNC frame and components (and any flex in the tool, particularly if it's long and sticks out a long way from the spindle) will upset front/back alignment
• You don't mention which kind of Shapeoko you're using, but I wouldn't trust any of the versions that use belts to be extremely reliable for this kind of work. Belts may stretch over time which will ruin repeatability and hence front/back alignment. Ball screws will yield more accurate, repeatable results for this kind of work.
• etc...

Many ways to skin the cat, but here's how I do it (assuming I've dialed in as much perpendicularity, rigidity and squareness into the machine before starting):

1. I use a dedicated fixture board that is rigidly bolted to the bed such that it cannot move. A simple G-code is used to machine four locating holes into the board at each corner outside the perimeter of the body that will be machined, plus a centre line is machined into the fixture board (MDF is OK). This only needs to be done once.
2. Using a sharp vee bit (60deg tip angle) I align the CNC tool tip with the bottom of the centre line on the fixture board and touch off X and Y axes as accurately as I can. Do not power-off or reset the machine.
3. Take body blank (assuming it's already as flat as possible with front/back faces as co-planar as possible) and mark a centre line. Extend the ends of the centre line down the edges too.
4. Remove the vee bit from the machine and clamp body blank on table, lining up the centre line marked on the blank with the centre line on the fixture board.
5. Install bit into spindle and touch off Z axis on the body blank.
6. Using the same code that generated the four locating pins in the fixture board (step 1) machine four matching locating holes into the body blank.
7. Remove the body blank from the CNC and install four pins (eg dowells, steel pins etc) into the four locating holes and align them with the four holes in the fixture board. They need to be a snug fit.
8. Run the same code that made the four pin holes in step 6 on the other side of the body blank.
9. Machine the body blank using your required tools and operations (can be either front or back - take your pick).
10. Once done flip the blank over, install the four pins on the other side and clamp to fixture board.
11. Machine the opposite side of the body blank using your appropriate tools and operations.

Using the above method I've been able to achieve alignment to within half a mm or less from front to back.

[mistermikev]

42 minutes ago, curtisa said:

Limit switches will only provide a relative reference for your machine for all subsequent operations. There are a lot of other ways for a front/back operation to fall out of alignment that limit switches alone will not correct:

• Backlash on axes (if any) cannot be compensated using limit switches and may result in the tool being further away from the commanded position than the CNC software thinks it is, which will translate to misalignment from front to back when the workpiece is flipped over.
• If the north-south travel (Y) is not perfectly perpendicular to the east-west (X) travel you'll see misalignment. Same problem will exist if the Z-axis is not perfectly perpendicular to the CNC bed.
• Rigidity of the CNC frame and components (and any flex in the tool, particularly if it's long and sticks out a long way from the spindle) will upset front/back alignment
• You don't mention which kind of Shapeoko you're using, but I wouldn't trust any of the versions that use belts to be extremely reliable for this kind of work. Belts may stretch over time which will ruin repeatability and hence front/back alignment. Ball screws will yield more accurate, repeatable results for this kind of work.
• etc...

Many ways to skin the cat, but here's how I do it (assuming I've dialed in as much perpendicularity, rigidity and squareness into the machine before starting):

1. I use a dedicated fixture board that is rigidly bolted to the bed such that it cannot move. A simple G-code is used to machine four locating holes into the board at each corner outside the perimeter of the body that will be machined, plus a centre line is machined into the fixture board (MDF is OK). This only needs to be done once.
2. Using a sharp vee bit (60deg tip angle) I align the CNC tool tip with the bottom of the centre line on the fixture board and touch off X and Y axes as accurately as I can. Do not power-off or reset the machine.
3. Take body blank (assuming it's already as flat as possible with front/back faces as co-planar as possible) and mark a centre line. Extend the ends of the centre line down the edges too.
4. Remove the vee bit from the machine and clamp body blank on table, lining up the centre line marked on the blank with the centre line on the fixture board.
5. Install bit into spindle and touch off Z axis on the body blank.
6. Using the same code that generated the four locating pins in the fixture board (step 1) machine four matching locating holes into the body blank.
7. Remove the body blank from the CNC and install four pins (eg dowells, steel pins etc) into the four locating holes and align them with the four holes in the fixture board. They need to be a snug fit.
8. Run the same code that made the four pin holes in step 6 on the other side of the body blank.
9. Machine the body blank using your required tools and operations (can be either front or back - take your pick).
10. Once done flip the blank over, install the four pins on the other side and clamp to fixture board.
11. Machine the opposite side of the body blank using your appropriate tools and operations.

Using the above method I've been able to achieve alignment to within half a mm or less from front to back.

so... first off - I appreciate that there is some good info here.  I hadn't thought of mentioning tramming, nor tightness of index pins, nor machine flex.

For context of my post op - I've learned a lot from curtisa and mikro.  their advice > my advice.  Really a novice here as I started cnc just a couple years ago.

many points that I instinctively use from above comments... for ex my spoil board is quality baltic birch and some 20+ (nylon) bolts.  when I built my spoilboard: I home my machine, setup/saved my offset, use a v bit to align initially.... drilled all bolt holes, then mounted, then drilled my index holes, then planed the surface.  that should all be relative to my offset.

but when doing index holes in my piece - I use a 3" bit to cut all the way through.  now... I've trammed my machine to .007 tolerance.  is there something i'm missing that you would drill index pins from either side as opposed to just straight thru.?  On the one hand that would avoid any error in the bit/collet... but if it's trammed that has to be a very small amount.

also... I mention backlash in my post.  and I say that homing is a correction for it, which your statement contradicts.  if I am wrong I'd like to understand why... but I was trying to point out that if you run a big 3 hour operation and potentially introduce some backlash error... you can then re-home and go to your offset - you'll be back to actual zero within the tolerances of your limit switches... effectively negating the backlash error. 

[curtisa]

Not suggesting there's anything wrong with adding limit switches to improve accuracy - it certainly does just that. But there may be some confusion as to what a repeatable home position actually does compared to backlash.

Backlash is primarily what happens when an axis reverses direction and there's a dead spot in the rotation of the stepper motor before the axis starts moving in response to the stepper's rotation.

Imagine the tool is at X=0. The software tells the machine to go to X=1. The axis motor turns, but because theres a bit of slop somewhere (loose coupling, stretchy belts, slogged-out leadscrews etc) the first couple of rotational steps of the motor does nothing to the axis until the slop takes up, and only then the axis starts moving. It eventually only makes it to X=0.98 but the software thinks it's at X=1. Depending on how bad the backlash is, including if it's asymmetric, the error can compound the further the tool moves from the starting position.

Adding home/limit switches makes home consistent, but doesn't help once the tool needs to move away from home.

[mistermikev]

1 minute ago, curtisa said:

Not suggesting there's anything wrong with adding limit switches to improve accuracy - it certainly does just that. But there may be some confusion as to what a repeatable home position actually does compared to backlash.

Backlash is primarily what happens when an axis reverses direction and there's a dead spot in the rotation of the stepper motor before the axis starts moving in response to the stepper's rotation.

Imagine the tool is at X=0. The software tells the machine to go to X=1. The axis motor turns, but because theres a bit of slop somewhere (loose coupling, stretchy belts, slogged-out leadscrews etc) the first couple of rotational steps of the motor does nothing to the axis until the slop takes up, and only then the axis starts moving. It eventually only makes it to X=0.98 but the software thinks it's at X=1. Depending on how bad the backlash is, including if it's asymmetric, the error can compound the further the tool moves from the starting position.

Adding home/limit switches makes home consistent, but doesn't help once the tool needs to move away from home.

so... not challenging at all... I just want to make sure I understand.  right so... machine moves to x=1 but has really only moved .98... then machine moves to x=0 but there is a different amount of backlash/slop-in-the-ball-screw... and it moves .9... now x=0 is .1 away from where it should be.  In theory this is all compensated for via an avg when setting your cycles/steps... and in practice on my machine it's not a measurable difference... as repeating a move against a dro... (admittedly w/o work piece resistance) I get the sm result multiple times... but in theory this could happen, no?

[curtisa]

41 minutes ago, mistermikev said:

s there something i'm missing that you would drill index pins from either side as opposed to just straight thru.?

Only that a shallower hole from each side runs less risk of being out of square than a single deep hole all the way through.

I should add that when I make the holes for the locating pins they're only 10mm or so deep. The pins are more like short nubs sticking up out of the fixture board.

[curtisa]

11 minutes ago, mistermikev said:

as repeating a move against a dro... (admittedly w/o work piece resistance) I get the sm result multiple times... but in theory this could happen, no?

If all the axis does is move forwards and backwards between the same two points all you'll likely see is that the overall motion will be shorter than expected by the backlash amount. A tool moving in a 1" square pattern might come out with 0.98" edges for example. But of course we do all sorts of weird curvy motions when CNC-ing a guitar body, so it gets weirderer quickly.

Depending on the software it might be able to enter backlash compensation values if you know how sloppy the machine might be. The software will then add extra steps to each change of direction to pick up the missing slack in the background. But you have to know what that slack is to begin with, which may be non-trivial to establish if you can't get your hands on the equipment to measure it with.

[mistermikev]

33 minutes ago, curtisa said:

If all the axis does is move forwards and backwards between the same two points all you'll likely see is that the overall motion will be shorter than expected by the backlash amount. A tool moving in a 1" square pattern might come out with 0.98" edges for example. But of course we do all sorts of weird curvy motions when CNC-ing a guitar body, so it gets weirderer quickly.

Depending on the software it might be able to enter backlash compensation values if you know how sloppy the machine might be. The software will then add extra steps to each change of direction to pick up the missing slack in the background. But you have to know what that slack is to begin with, which may be non-trivial to establish if you can't get your hands on the equipment to measure it with.

right on, I appreciate the answers as always.  I'll stop derailing the thread now lol!  thank you thank you.

[jeremiah.peschka]

This is all awesome information. Thank you both.
 

There's definitely no derailment here, I'm learning a lot from everything written above.

[curtisa]

Another approach you can take if front/back alignment is an issue is to avoid trying to do it in the first place.

When you think about it, there's only a handful of machining operations you actually need to do on the rear of a solid body guitar - the control cavity, the spring cavity for a trem (if present) and the belly cut. 75% of the work is entirely from the front. You could do the pickup cavities, neck pocket, pot/switch holes, bridge holes/cavity and body outline to a depth of 10mm or so from the front, cut away the half-machined body from the blank using a bandsaw and then use a bearing bit on the router table to remove the remainder of the body outline manually. Alignment of the body edges from front to back would then be a non-issue.

The rear operations can then be done separately without having to worry about getting alignment perfect - It probably isn't a huge issue if the control cavity is off by 1/8" compared to the front, and the belly cut could be done entirely by hand using a rasp if you really wanted.