Official Luthiers Forum!

Hey everyone.

I am having an odd issue while trying to cut out guitar neck tenons. The tenons have 2 fretboard locating holes on the top, and the cut out edges of a neck tenon.
The locating holes are cut with a 0.25" router bit and the edges of the tenon cut with a 0.5" router bit.

The measurement from cut outter edge of neck tenon to the fretboard locating hole edge should be 0.618" on each side.
On the numerous test pieces I have done, I repeatably get something like 0.599" on one side, and 0.630"-0.640" on the other.
The only time I have managed to minimize that error (to within 0.010") was turning the whole toolpath 90 degrees, or, using only one tool (0.25" router bit) and doing all the cutting in one operation.

My code is fine when you retrace in CAD what it is doing movement wise. My steps per is fine.
I even had someone else try my code on their CNC, and it produced the same error.
*I can't figure out how to attach my code on this forum. It keeps saying it is not allowed.*

I can't figure out what would be causing this issue.

Try posting pictures. Super hard to visualize what you are talking about.


Sent from my iPhone using Tapatalk Pro

Perhaps your zero isn't where you think it is?

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

Here are some Photos:

Measured from inner tenon edge to closest edge of fretboard locating hole.



Another example cut into a test piece:


The one on the bottom of this image has the toolpath flipped 90 degrees. This made the outcome a lot more accurate (within 0.01" from one another). The one above it, done with only a 0.25" router bit and all finished in one operation. No tool change, no second toolpath for the 0.5" router bit.



I have checked my zero location. (the machine is homed after every tool change) So I don't think that is the issue. But obviously, I can't figure this out so I am open to any and ALL criticism and ideas.

I think the next diagnostic step is to cut like a 1" square and measure it to see if that cuts accurately along both dimensions.

Some other things that come to mind without knowing anything else about your situation:

1) Your machine might not be rigid enough to hold the accuracy you're after. With a flexy machine climb and conventional cutting will change dimensions.

2) Your home switches aren't very accurate.

3) Your CAD model is off and you haven't realized it.

4) you have backlash or a loose pulley or something like that.

An error of .010 is very very high.

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

Hey Andy, thanks for responding.
Here is a 1", 2" and 3" square test cut:

1) Your machine might not be rigid enough to hold the accuracy you're after. With a flexy machine climb and conventional cutting will change dimensions.
This definitely could be. My machine is an old Isel (Techno) CNC. There is not much information but, the link to it is here: http://www.techno-isel.com/Tic/H830/HTML/H830P046.htm

2) Your home switches aren't very accurate.
I was able to measure my home switches to be within .0005" with a dial indicator

3) Your CAD model is off and you haven't realized it.
This also could be possible but I have checked it a million times (I feel like I am losing my mind here!). If I was able to supply my Gcode, do you think you could have a look at it, or even test it?
If you don't get the same discrepancy I do, then it must be the flexing in my CNC.

4) You have backlash or a loose pulley or something like that.
This could be. Wouldn't my square test cuts show this as well though?


I look forward to your reply.

Your machine is almost certainly stiff enough for this application. I'm kind of scratching my head here.

I don't really have time right now to run a test and just looking at G-code can be really frustrating to figure out what's going on.

The square cuts should verify that backlash or loose pulleys.

I'm kinda leaning toward a CAD mistake but you said you've checked it many times. What software are you using?

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

I am using Mastercam X4 for CAD and CAM.
If you can find some time, I would really appreciate it.

I have been chasing this issue for quite some time now and I can't seem to figure out why the heck it would do this.

I have even taken my Gcode and traced out the moves in mastercam to see if something messed up is happening.
When I finished the drawing in mastercam from just the Gcode measurements, the drawing was perfect. There was no discrepancies in measurements.

Hi Alexander,

I wish I could help more but as a fellow professional, I think you can understand how valuable time is - In addition to being a little behind on paying work, I'm super behind on non-paying type of work (machine upgrades, maintenance, website, cleaning etc) and I simply can't afford to take this on at this time as a freebie.

Try re-drawing a simple 2.5D version of the same thing and see if you get the same results. If you do, it's something to do with the machine. If you don't it's something with the model.

Something I didn't mention before is controller type stuff. Mach 3 is notorious (at least among those of us in the know) for having a horrible trajectory planner and if you're using that for control, it could possibly be the issue. Your "square test" implies that your CV mode settings are good, at least for sharp corners but, I've had Mach 3 screw things up for me royally on certain parts with settings that worked fine for other projects.

Check the following and compare it to your model:

Is the width of neck at the heel (widest point) accurate and does it match the model?
Is the truss slot centered?
Are the holes equidistant from the truss slot?
Look for any G41s or 42s in the code. If they're there, that might be your problem.
Look for a G40 in your code. If there's not one and you're not using cutter comp, you should add it to your header line

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

This is a small point, but isn't it better not to home the machine between tool changes unless you're switching to a new workpiece?

What kind of homing switches do you have? I think most mechanical switches can have inconsistent points in their travel for when the circuit is opened.

I've been taught that if you're concerned about losing position between tool changes then it's better to recheck zero first before homing the machine. Reason being that unless the homing switches function with extreme precision then they are likely to introduce drift.


All that said, if you have servos and a control box which can return each servo to an exact position in it's rotation when homed then you should be able to disregard everything I've said above.

Ah looks like my previous post is probably not helpful at all.

I should have read the thread more carefully first!

You boxes are square, so that seems to indicate the machine is unlikely the problem. The dimensions of the neck are correct, right? So logic dictates that something about how you are doing the drilling operation is off. It’s the locating holes that aren’t where they should be.

Using the same cutting strategy, what happens when you drill a grid of holes? I would suggest using a v-bit to trace a checkerboard and then drill the exact same locating pins with the same bit/federate/strategy at the intersections. Are the holes where they are supposed to be?


Sent from my iPhone using Tapatalk Pro

Awe heck. If you send me a test file I'll run it for you. Just don't send the whole thing, send me the small one that just cuts that little bit. You can either contact me through the website or shoot me a PM for my e-mail.

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

rlrhett, I never thought of that... Maybe my locating holes are to blame and it is not the cutout. I don't have any v bits, but I will try and acquire one to test.

Andy, I really appreciate you making the offer to do the test. I have emailed you through your website.

Mine came out just about perfectly but I think I know what your problem is: your stock is moving during the 1/2” cut



Mark your table very carefully with a scribe or pencil or something and check it out. Your spindle speed is quite low for that cut in my opinion. I’d normally cut that about 15k to reduce cut ting forces.



Sent from my iPhone using Tapatalk

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

So?

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

I have been meaning to reply.

I ran the spindle at 15k for the 1/2" cutter and I still have the same issue. I also bolted the piece down to the table to try and minimize as much possible shifting as I possibly could.
This test also produced the same results of 0.599" on one side, and 0.630" on the other.

I am at a loss of words!

Wow, Andy did some really nice work for you ! Sending him one of your strong Canadian beers might be nice.

I have one of those Techno machines, mine still has the stock servos and controller, you are on steppers and Mach3 ?
They are not very rigid, especially when doing any kind of heavy cuts/slotting in hard wood like maple. Nothing is very
straight or square on my machine. Putting a dial indicator in the spindle and pushing gently on things causes a lot of
movement in the indicator because the thing just has a lot of flex. It can still be a useful machine.

Since your cuts using a .25" EM are acceptable it's either the extra cutting forces from the .5" EM or something funky with
how the controller is dealing with that bit. Are you doing machine comp ? Any G41's in your code ? Look at your D? and
wear in your tool offsets. Try posting without compensation, there must be an option in Mastercam for that. Comp should
be doing the same thing on both sides of the heel but comp needs lead in to work and I can't see what you are doing there.
Some controllers will just ignore a G41 if the lead-in requirements are not met, others will error out.

Regarding machine flex, you look like you are trying to slot your way around the heel in one go. Do an overcut leaving say
.015" and then do a finish cut to size. That way the actual cut to size is only taking .015" worth of material and there isn't
the cutting forces to cause as much flex. Using a chipbreaker spiral will greatly reduce the cutting forces on your machine and
still give a good finish quality.

Once you get things running right, try to enable compensation so you can cut to spec dimensions more accurately. I've learned
that most bits are not accurate to size, especially "router" bits are intentionally undersized to accommodate runout from router
spindle bearings. My Renishaw toolsetter measures this stuff and they are all over the place even from the same manufacturer like
Onsrud. Metal cutting bits are more accurate. Use your diameter / wear registers to dial in your actual bit diameters.