want to get feet wet... looking for recommendations

[MiKro]

7 minutes ago, mistermikev said:

ima b honest.... kinda blurry but... looks like some nice figure. 

A piece of scrap I found laying in the back of the shop. LOL. This is going to be a neck for a CBG 3 string. 

mk

[MiKro]

So to speed things up just a bit, I tried using a smaller number in my meshes/breps. which in turn creates larger triangulations if converted to STL. This is not good. While it may look good in the software design, it shows up on the CNC as large triangulation and is rough, So I will need to go back and redo this one.

Since it is a one off I will just sand the neck. but it does make me look at my settings in Rhino.

MK

 

 

[mistermikev]

2 hours ago, MiKro said:

So to speed things up just a bit, I tried using a smaller number in my meshes/breps. which in turn creates larger triangulations if converted to STL. This is not good. While it may look good in the software design, it shows up on the CNC as large triangulation and is rough, So I will need to go back and redo this one.

Since it is a one off I will just sand the neck. but it does make me look at my settings in Rhino.

MK

 

 

wow, that's a lovely piece of scrap.  if I may - what bit do you use for the finished pass?

[MiKro]

14 hours ago, mistermikev said:

wow, that's a lovely piece of scrap.  if I may - what bit do you use for the finished pass?

I was using a 1/4" ballnose with a 6% stepover at 180ipm for this. My finish pass endmills are determined by what I am doing.

[MiKro]

So when you use Aspire and some other types of CAD/CAM software that import STL files mainly. This is the problem you may face with STLs. If the mesh count is not up to par it will introduce triangulation artifacts in your work. Which will show up in the milling as well. Sometmes in Aspire you need to up the visual resolution in order to see it.   There are also two available higher resolution modes, Extremely high (20X slower) and Maximum (50X slower) that are not normally visible. They can be made available in the Model Resolution pull-down menu by holding the Shift key down before selecting Create a new file or Job Setup. This can be very useful when needed.

So to give an example look at the neck transistion to the headstock. One has low mesh count the other high mesh count. Both are the same file only mesh sizes changed in Rhino before export.to STL for use in Aspire.

I experienced this myself by cutting corners in Rhino to make a quick neck model for a Cigar Box Guitar.

MK

 

 

[mistermikev]

53 minutes ago, MiKro said:

So when you use Aspire and some other types of CAD/CAM software that import STL files mainly. This is the problem you may face with STLs. If the mesh count is not up to par it will introduce triangulation artifacts in your work. Which will show up in the milling as well. Sometmes in Aspire you need to up the visual resolution in order to see it.   There are also two available higher resolution modes, Extremely high (20X slower) and Maximum (50X slower) that are not normally visible. They can be made available in the Model Resolution pull-down menu by holding the Shift key down before selecting Create a new file or Job Setup. This can be very useful when needed.

So to give an example look at the neck transistion to the headstock. One has low mesh count the other high mesh count. Both are the same file only mesh sizes changed in Rhino before export.to STL for use in Aspire.

I experienced this myself by cutting corners in Rhino to make a quick neck model for a Cigar Box Guitar.

MK

 

 

hehe... you are my yoda.  as it were... I'm going to be facing this issue shortly I suspect as I transition to neck design for my bass.  Further... current graphics card is being pushed to the limit on standard resolution... but we will be rectifying that shortly.  (nother side proj coming up - building a 16 core pc!!)  I will come back to this thread once I get there and I'm thinking this will be very relevant then!  thank you for that!

afa bit... just wondering if you are in fact going down to a tapered ball nose 1/8" bit for finishing.  it appears to be the recommendation but will result in an estimate run time upwards of 10hrs!!

[MiKro]

2 hours ago, mistermikev said:

>snip<

afa bit... just wondering if you are in fact going down to a tapered ball nose 1/8" bit for finishing.  it appears to be the recommendation but will result in an estimate run time upwards of 10hrs!!

I only use those on very fine work. I have even used 1/16" and 1/32" TBN, Otherwise I use a straight 1/4" or 1/8" BN. One other thing is not to do all of the surface just what needs to be milled using  a vector to contain the area. If it is flat there is no reason to mill that in a finish. it can be easily sanded to transition if needed..

MK

 

 

Also the back side ready to flip.

[mistermikev]

1 hour ago, MiKro said:

I only use those on very fine work. I have even used 1/16" and 1/32" TBN, Otherwise I use a straight 1/4" or 1/8" BN. One other thing is not to do all of the surface just what needs to be milled using  a vector to contain the area. If it is flat there is no reason to mill that in a finish. it can be easily sanded to transition if needed..

MK

 

 

Also the back side ready to flip.

right on.  using a 1/8 ball vs 1/4 ball makes a huge dif in the time estimate it comes up with.  Also, I've noticed that the whiteside .tool database bits are set to run much faster and as such come out with much lower time estimates.  I figure I'm going to be doing plenty of sanding so I'll probably just go with a 1/4 ball nose and call it good enough. 

afa area... right now I'm just working on the body... and everything is restricted to the bounds of the body in 90% of the area.  I will keep that in mind tho - no sense wasting bit/time/etc on something that doesn't need to be carved.

that's a nice clean edge where that neck meets the heel.  I love that about cnc... just looks so professional.  nice work.

[MiKro]

So now I have flipped the neck blank. and resurfaced it just to the point of opening up the heel cut.

Why you ask? This way I can now cut the slot for a truss rod, add the fretboard blank with a rear over hang for a 24 fret. Next will be to radius the Fboard after making the markers. Then I will cut the fretslots with the radius . then scallop the headstock which I already drilled the tuner holes when it was on the other side. last I wil profile the entire thing including  the fretboard overhang. I have already profiled the neck heel from the other side.

 

[MiKro]

So back to the CBG neck. I used an old fret board I had laying around and epoxied it to the neck blank after installing some POS truss rod I had laying around.

I got in a hurry and forgot to put a spacer on the top of the truss rod adjustment area. I would usually mount this type being heel adjust but being a 3 string and all I went easy.

I radiused the board to 18" and then the head stock transition. All in all okay. Need to layout markers since I had already slotted the board many years ago and forgot to do it before radiusing. LOL.  Yep stupid me. The booze was good though.

Just sitting  back having a drink doing stupid stuff while the machine ran. With out the insert for the truss rod it looks weird but what the fuck it is a toss around Shop 3 string. LOL

UPDATE: Well when I screw the pooch I do it very well. LMAO!!  I measured the wrong damn fret for the location to set the markers, so you guessed it. Scrap one fret board. LOL!!!

 

.mk

 

Starting over with the fret board. LOL

 

 

[MiKro]

I don't know what I have been thinking? I was going through a bunch of old stuff. Found some old Strat Necks that are already done with paddle heads

I think I will just fixture one up and trim the damn thing to make a CBG neck quick. LOL!!

MK

[mistermikev]

hehe, nos guitar necks - I'm told they are all the rage... very "in" right now!!  

[MiKro]

1 hour ago, mistermikev said:

hehe, nos guitar necks - I'm told they are all the rage... very "in" right now!!  

I think these are some chinese specials that someone had that I got in a buy out. LOL.

I also found a complete Carbon Fiber neck that was in the group. LOL Funny how when cleaning shit you find shit.,

mk

[mistermikev]

Just now, MiKro said:

I think these are some chinese specials that someone had that I got in a buy out. LOL.

mk

so... n.o.s. chinese fender knecks.... nice. hehe

[MiKro]

1 minute ago, mistermikev said:

so... n.o.s. chinese fender knecks.... nice. hehe

perfect for a CBG LOL

mk

[mistermikev]

Just now, MiKro said:

perfect for a CBG LOL

mk

tru dat

[mistermikev]

so I come here to chew bubblegum and piss and moan... and I'm all out of bubblegum.

so, still issues with my machine cutting a neck pocket.  have had some help here from mikro - went through my machine and tightened all couplers/bearings and ruled that out - did make some improvements but were not quite there yet.

I've cut out the body shape, the pickup cavity and several other projects - all with no issues... but the neck pocket - if I start cutting it and stop the machine and go back to zero: I'm no longer at zero.

had some help from a gent on cnc6040 group on facebook, he generated a tool path for me to rule out my cad/cam... funny but that tool path causes the x to drift in the opposite direction!  ie sm problem in reverse.

so at this point... I figure I must be losing steps.  I'm thinking a whole lot at this point about things from getting a planetcnc card ($70) and replacing just my motion control breakout board and using their version of mach3... to buying the parts for a gekko g540/power supply/vfd/wire and building a whole new controller ($500-$800). 

needless to say my dreams of cutting a neck pocket are no where in my near future.  I don't think I'll even bother trying to run the cnc for the body contour/3d stuff.

 

Mostly I just want to piss and moan.  Sort of surprised that what I thought would be "the learning curve" was going to be learning cad/cam/mach3.  Not that I'm particularly great at those things but they haven't posed nearly the challenge that "random mechanical problems" have.

there... I feel better.

[MiKro]

Mike,

Mach3 is not your problem unless you have inadvertently set something incorrectly. 

Are you positive that the steps are set correctly? If not sure at minimum run the auto set feature for each axis. Use at minimum a good set of calipers to measure and set this. Go to at least 5" or more if your calipers will allow.

Have you checked for backlash in each axis? If not then remedy that.

Have you checked for squareness of x and y? Also perpendicular Z to each of X and Y (tramming) ?

I hear this all of the time from people. It is Mach3, or it is Aspire, or what ever software. 99% of the time it is a mechanical problem, a setting that is wrong, or EMI electrical issues.  If it is software related, 99% of the time it is the user has made a mistake in the software use.

Just my many years of use and helping others with problems, experience.

Basically my 0.02cents.

Mike

 

 

 

[mistermikev]

10 minutes ago, MiKro said:

Mike,

Mach3 is not your problem unless you have inadvertently set something incorrectly. 

Are you positive that the steps are set correctly? If not sure at minimum run the auto set feature for each axis. Use at minimum a good set of calipers to measure and set this. Go to at least 5" or more if your calipers will allow.

Have you checked for backlash in each axis? If not then remedy that.

Have you checked for squareness of x and y? Also perpendicular Z to each of X and Y (tramming) ?

I hear this all of the time from people. It is Mach3, or it is Aspire, or what ever software. 99% of the time it is a mechanical problem, a setting that is wrong, or EMI electrical issues.  If it is software related, 99% of the time it is the user has made a mistake in the software use.

Just my many years of use and helping others with problems, experience.

Basically my 0.02cents.

Mike

 

 

 

I agree that it is unlikely an issue with mach3... wasn't suggesting that... just thinking about replacing the controller with literally 'anything' else as I'm told this controller is not great and that this issue is likely related to grounding issues that are common on this machine.  there are many threads about gutting them and replacing the controller and all wires.  I don't want to go to that extreme... and I'd love to rule out everything else first.

I bought a dial indicator and an arm for doing just this (calibration)... but got stopped when I realized I didn't have a way to mound it in my collet (it's too big) and then realized - aluminum is not magnetic (hehe) so can't stick to the bed.  I need to rig up something to overcome this and will do for sure asap.

can you elab a bit on backlash?  I think that would just be an issue if I was running in wood right?  I'm literally running this above my work piece in air and observing it go off course.

I have my work-piece setup exactly parallel with the y axis.  I've jogged to one end then the other with a 60deg engrave bit and it is on the line exactly at either end.  that said... when I run this program it will pull zero out by .5" in a matter of 30 seconds.  No other programs will.

Now, I've cut several things and come back to zero and we're spot on... but if I cut this neck pocket for a few seconds... and go back to zero - we are way off.

I appreciate your help and don't want to abuse that - super valuable to me.  your .02 is worth it's weight in gold to me so thank you.

[curtisa]

Could be mechanical - lost steps or a loose motor-to-leadscrew coupling is a possibility if the drift is only in one axis. Is this neck pocket routine particularly aggressive in terms of the cuts being made? Are there lots of hard corners in your routine where you're asking the cutter to make 90 degree turns while deep in the workpiece?

Backlash is usually only going to show up as a consistent small error when reversing the direction of an axis; squares that come out looking like rectangles or circles that look like ellipses. But we're usually talking about a mm or so of difference at the most. Half an inch of loss of positional accuracy in 30 seconds of motion is unlikely to be due to backlash.

[curtisa]

The other option if all your toolpaths work fine except for the neck pocket is that the neck pocket code has something in it that upsets the X axis zero. Maybe you have a couple of moves programmed in G91 incremental mode that aren't being cancelled properly, or a G92 coordinate offset accidentally enabled?

I'd regard total replacement of the motion control hardware as a last resort. Replacing the entire drivetrain of your car because one tyre goes bald quicker than the others seems a bit excessive.

[mistermikev]

1 hour ago, curtisa said:

Could be mechanical - lost steps or a loose motor-to-leadscrew coupling is a possibility if the drift is only in one axis. Is this neck pocket routine particularly aggressive in terms of the cuts being made? Are there lots of hard corners in your routine where you're asking the cutter to make 90 degree turns while deep in the workpiece?

Backlash is usually only going to show up as a consistent small error when reversing the direction of an axis; squares that come out looking like rectangles or circles that look like ellipses. But we're usually talking about a mm or so of difference at the most. Half an inch of loss of positional accuracy in 30 seconds of motion is unlikely to be due to backlash.

thank you very much for the response. 

well, good advice there - it is exactly what Mikro advised.  I went through my machine, and tightened all the leadscrews.  x was a hair loose... but it didn't solve the issue.  I also tightened the linear bearings (I think that's what they are called) and it make everything a bit tighter and yet still smooth... but didn't solve the issue.

yesterday... on a whim I added some ferrite beads to all axis... when I ran immediately after - it actually ran right... but then ran again to see if it was consisten and it ran wrong.  this makes me think it's def a noise issue on the cable. 

was running this in air and getting these issues.  my shape does have two square ends that are actually outside the body area... and I could easily change them to rounded corners... but I don't know how that could cause the issue.

24 minutes ago, curtisa said:

The other option if all your toolpaths work fine except for the neck pocket is that the neck pocket code has something in it that upsets the X axis zero. Maybe you have a couple of moves programmed in G91 incremental mode that aren't being cancelled properly, or a G92 coordinate offset accidentally enabled?

I'd regard total replacement of the motion control hardware as a last resort. Replacing the entire drivetrain of your car because one tyre goes bald quicker than the others seems a bit excessive.

well, I had a more experienced cnc'er create a toolpath for me in a completely dif software.  oddly, it caused the x axis to go off more and in the opposite direction!!  funny thing is... I had re-written the toolpath to do a east/west raster... and this stayed pretty much on coarse until it got to the final pass where it does the profile... then blew up.  so it doesn't seem like it's even an east/west issue, but more an issue of combined easte/west while running north/south. 

afa total replacement - you are def right on here.  I've since reconsidered this and am going to have a good look at it tonight... and possibly start by replacing the motor wires.  I've read quite a bit on the forums re the 6040 and this is the common theme on them.

further, at some point - I'd like to replace the controller anyway... as I'm told the improvements in stability and rapid speed are immense... so that was part of the motivation of a knee jerk reaction to replace everything.  i figure, if I'm going to get in there and have to jack around improving the grounding... might be just as much effort to build something new.

so... with your cnc... 20 questions... did you have usb or parallel?  what controller board did you have?  did you use mach3 or something else and if so what?

[MiKro]

4 hours ago, mistermikev said:

>snip<

I bought a dial indicator and an arm for doing just this (calibration)... but got stopped when I realized I didn't have a way to mound it in my collet (it's too big) and then realized - aluminum is not magnetic (hehe) so can't stick to the bed.  I need to rig up something to overcome this and will do for sure asap.

can you elab a bit on backlash?  I think that would just be an issue if I was running in wood right?  I'm literally running this above my work piece in air and observing it go off course.

>snip<

A dial indicator is help for tramming not really for step length. I use DRO's but they are expensive.

I used to use a digital caliper. Make a straight line cut about 1/8" deep. Say 5" long. Start by moving the mill a short distance in the direction of the first cut as this will load the ballscrew correctly for that measurement.. Then measure the actual length of the cut minus the measured value of the cutter diameter. This will be what it is actually doing or very close. then compare to what the step settings are? Do not do it both ways and use that measurement it will be wrong ( it will have backlash in this measurement). Get this correct first before looking at backlash.

Next with out moving anything other than Z up some for clearance after making a cut as described above. Now make the same cut next to it by moving the other axis only first ( do not unload the first cut movement. Now Go the opposite direction cutting and measure that. Now you will see your backlash amount in the screw/ballnut for that axis. Only do that part after you get the true length correct.

Hope that makes some sense?

MK

 

[mistermikev]

44 minutes ago, MiKro said:

A dial indicator is help for tramming not really for step length. I use DRO's but they are expensive.

I used to use a digital caliper. Make a straight line cut about 1/8" deep. Say 5" long. Start by moving the mill a short distance in the direction of the first cut as this will load the ballscrew correctly for that measurement.. Then measure the actual length of the cut minus the measured value of the cutter diameter. This will be what it is actually doing or very close. then compare to what the step settings are? Do not do it both ways and use that measurement it will be wrong ( it will have backlash in this measurement). Get this correct first before looking at backlash.

Next with out moving anything other than Z up some for clearance after making a cut as described above. Now make the same cut next to it by moving the other axis only first ( do not unload the first cut movement. Now Go the opposite direction cutting and measure that. Now you will see your backlash amount in the screw/ballnut for that axis. Only do that part after you get the true length correct.

Hope that makes some sense?

MK

 

well that's a good idea... testing it under load as opposed to not.  that is a solid idea.  wish I'd have known that before I bought a dial indicator! 

don't see how this corresponds to step tho... I was under the impression that step was a pre-determined measurement based on your motors... and that for the 6040 it should be 320.  So the mach3 calib where you tell it to move 1" and then measure and enter that value: that changes steps?

[MiKro]

Here are the steps for auto step calcs in MAch3.