My new Shapeoko 3 is it just me?

[Rocket]

It cut through .25 ply..

That is not the problem, when I make a gear in
Gearotic, post it, and load the code into Carbide Create
it makes a mess of the output.

Gear looks like it was made with a hammer by a 3 old....

Could I get a Pokey usb cnc board and change over from
the Carbide board?

[Nate]

It may be helpful if you post a picture of the bad gear.

[Richard Cullin]

my point is that if you overload the machine by cutting too deep or too fast or both then that distorted gear is the result.

you need to establish some working parameters for your machine first
how fast how deep what spindle speed work with what material you are trying to cut

its like towing a trailer home with a Toyota corolla versus a f300 pickup  , with the corolla you need to slow down and be much more careful

[ArtF]

Rocket:

I wouldn't recommend changing anything, not until your quite familiar with what youre doing
and can run jobs. While the hardware isnt top end, its not bad. The electronics, though a bit weak isn't
so bad you need to do anything. The software , this "carbide", is truly horrible, but again workable
though only barely.
  You need to figure out what exactly is bothering it in the text, and fix it. Id think the
makers would be happy to help. Id just keep in mind, down the road when you DO have it all working
and understand the issues, that you probably DO want to replace its electronics. The software
choice and electronics choice they made in design was a bad one IMO. Its making an acceptable
machine into a rather cheap copy of a useful cnc device. (All this is only my opinion I might add,
and based only on looking at their software and exploring their forum. My apologies if this
makes any shapeoko users feel bad, its not my intent, but I think your wondering just
what I think, and I don't think Id be doing you any favor by praising the unit as I see it. )

  It would take a pokeys 56 or 57 and 3 stepper drivers. All told probably a couple hundred
bucks and a bit of wiring. That however, would make the machine orders of magnitude more
capable and useful. You could run Mach3, Mach4 or Auggie on it at that point. Youd have graphical
displays of the loaded file and what will happen when you run it, and it really helps in understanding
whats happening. It ISNT however, something to do when your not familiar with G code and how a machine
works.
  My advice, find out whats wrong, ask them , and us, when your wondering on something. Fix the trouble
by finding what you need to edit, its likely its only one line its choking on or doesnt understand.
Then , when you've cut a few gears and your familiar with things, look at an upgrade and get rid
of that silly program. Whether you go Mach3, or Auggie, you'd be magnitudes better off.

           But really, do not do this until your ready or feel you are. What you have CAN work, though you may
have to edit files from GM to make them work. If you find the problem I can probably make a post change for you
to make the files work directly when posted, or at least in a condition where you know what you have to do to make
them work.

 So look at it as a learning exercise, you just got a wooden flute, learn to play it before you turn it into
a digital synth that makes any other sounds you may want. Your mechanics look pretty good, not great,
but Ive seen much much worse do great things, your software is all that's holding you back, it will simply
take a bit of work to figure out how it works on normal GCode files.

 Good news is they use Meshcam, a very good program, and Rob , back when I dealt with Meshcam as
one of my OEM's was a great guy to deal with. So the makers of shapeoko must have some idea as to what
Gcodes are messing it up and it messed up with both Meshcams files as well as Gearotics. ( And I assure
you both programs put out good cutting code. ). So the problems are likely known, and Im sure other
users of that machine can help you with what is wrong with the Zeroing or code run.

 Yell when you have questions, Im not very particular about what someone is using, Ill help where I can
on any topic I can, and others will kick in as well when they see something they wish to straighten
you out on.

Art

[Rocket]

Art...this may sound simple, but you are a good man.
There are not many left on this earth.
Thank you.

There is a dealer here in Florida that sells Pokeys...he is about 40 miles north of me.

I will call them tomorrow and see what they have.

https://www.cnc4pc.com/

I grew up as an electrician, wiring would not be a problem, spending 200 is okay if
it frees me up to get some fun work done and not messing around with this Carbide Software.

RR

[ArtF]

Rocket:

  The guys at cnc4pc are pretty good by all accounts, and they know of what they speak. Forum posts
are a terrible way to get a good feel. Discuss it with them as much as you can.  I suspect
putting in a pokeys 56, and 3 stepper drivers isnt out of your abilities, but again... I really recommend
you stick with what you have until you KNOW the problem is that you need to take light cuts,
or the GCode for M30 is screwing it..or whatever it is.
  As Richard says, test and test again. KNOW what the issues are, THEN address them. The guys at
cnc4PC will not steer you wrong, they know CNC in terms of Mach3, and can make your machine quite
useful. But it will help them if they KNOW what exactly your issues are,on the other hand they
may already know your machine and can advise. Tell them they came recommended.They may even
remember me. :)

Art

 

[ArtF]

Rocket:

  Ask the Guys at CNC4PC, ( Arturo Duncan I believe), if they can show you a wired machine and software
running it, just seeing it all in one place would undoubtedly help you out a lot. Worth the
trip just to see how it all works if you don't mind the travel.

Art

[Rocket]

Good info.

I was up at 130AM.

I am so excited about this new accomplishment even though
it is not perfect, I think a few more tweaks and I may have IT!...well partially anyway.

I made this small 4 inch gear in your great program, played around with the g code a little
(I sound like a programmer...NOT EVEN CLOSE).

Slower everything down...feed-rate of 10.  4 passes with a .0625 end mill, 1/4 inch plywood (pine).

As you see in the photo it almost worked.  (the part that is missing is not an error, it is
overlapping a previous cutout...same material when we can.

Here is the g code, I am sure you can tell me why it is not perfect.

Attachments:  G-code and JPG of gear.

I wish I could meet you....

Spent about 5 summers in Whistler, but my friend sold his
home there a few years ago........beautiful........

Rocket

[ArtF]

Rocket:

  I think your there. :)

  GCode looks good, I think the main issue was too much cut per pass.
How much per pass you can use is a function of stepper power, and spindle power.

Few more tests and I guess your on your way. :)

Congrats.
Art

[Rocket]

Thanks....

You cannot see it in the picture, but it cut a
path from 0(zero start) to the first real cut in the job.

In other words after I zeroed it out before the job started,
instead of z-axis going up to travel to start point it just started
cutting a zero mark?

I cannot find the setting in Gearotic to tell the machine lift the spindle
while traveling to the start of job.

I hope I am saying that right.

R

[Rocket]

Art,

You say: GCode looks good, I think the main issue was too much cut per pass.

If that is the case how do you explain why it cut the first 3 inside profiles okay
with each one doing (I think) 4 consecutive passes?

R

[Rocket]

Art,

What do you make of this?  It started perfect
for almost 2 hours....(is that a very long time).

RR

[marklazarz]

Rocket:

How are your parts clamped or otherwise secured when you are machining?  It sure looks like something is moving by your photos.

Also, are you using sharp cutters capable of proper chip removal?  Instead of an 0.0625 end mill, try to cut a larger gear using a 0.125 or 0.1875 sharp straight two flute bit and see what happens.

Mark

[ArtF]

Rocket:

  Looks to me like the wood is moving.. or, much more likely, your losing steps. One
or the other is certainly true.

  First, lets talk about that path to the first cut. If your zeroed at the top of the material, the Z should lift
up to whatever you have set in Gearotic as "Safe-Z" before it moves. When you generate a
file, make sure SafeZ is set to a positive number, in your case about .25 or so, that makes it move 1/4" above
the material between cuts. Moves between cuts are made at rapid speeds, so if your in the wood when it moves
to the next cut, you will lose position.

  Try it that way and see if it screws up the same, if not, it was trying to drive at rapid while in the material
that was the issue, if it still screws up, you need to then see whats moving. Stop it hapf way through as tell it to jog back to zero. It is returning to the original zero? If not, you lost steps. That means an even lower depth per pass setting is needed.

  You asked of time, a 5" gear in .25" plywood would take my Mach3 wood router mill about 5-10 minutes typically,depending on depth
per pass and diameter of tool. It looks to me like your gear started to cut properly, then lost steps. (Or the material moved.)

Another note, the smaller the tool, the less likely this happens.To cut a 5" gear, Id use a 3 mm tool diameter, runs fast and is small enough to fit in the teeth. You generally use the smallest too l you can for a given job.

So, try another lower the depth per pass, and see what it does. If it starts to screw up, stop it and jog back to zero, is it off?

  Two hours on a 5"  1/4" plywood gear wouldnt be considered slow, it would be considered to be an abomination. BUT, it is what
happens if way underpowered or going way too slow.

  What feedrate did you end up using? can you post that Gcode file here so I can double check Im not missing something.
Id be using something like 3000mm/min or so here I think were I do to .125 per pass in plywood, thats about F100 ,
and mine is not a real high quality unit, but it has good steppers, drivers and mechanics. Were I doing .125 passes,
Id up it to F200 maybe... I mention this just to give you an idea of how bad thats working.
Check all your linkages from stepper to drive pulleys, mark the shaft with a marker and check periodically to see if they slipped.. Somethign is very badly wrong, OR that machine is very very underpowered for its drives. I find it hard to believe it wont do
F10 at .125 in plywood, F50 in hardwood should be possible, let alone an F10 in plywood.
   
  Is your spindle struggling? You shouldnt go so fast it struggles, if my spindle slows, Im going tooo fast. A
spindle thats struggling will negate the power of the drivers and mechanics, you must never go so fast the spindle
is struggling.

  Heres my advice, You need to make line cuts to see how fast it can do without trouble, make that square
we discussed and do it at higher and higher F rates.. See where it stalls at and when the square becomes
a non square.

  Your getting there, its incremental and your now at a spot where testing makes sense, a lot of it.
Document the tests, you forget fast. List it on paer, Im OK at F2, F10, F20 F15 starst to go bad..

Im OK at Z-.125, Z-.1 ..etc..

Show us the results, and we'll tell you whats wrong. :)

Keep at er..

Art




   


   


 



 

 

[ArtF]

Rocket:

A couple more thoughts since your probably trying to consider everything.  Consider
what the drives see as they push through wood, basically exactly what youd feel if
pushing a router through wood. You want your router running real fast, like 20,000RPM
to make that router slide though the wood like butter, get the speed of the spindle
too slow, and its like pushing though denser and denser material. Spindle speed is a very
important consideration. Steppers have good power at low speed, their torque decreases
with speed, so making sure the router or spindle is seeing no more than butter in front
of it is very important. Obviously size of the bit also has the same effect, smaller the better.

So, if I assume your using a laminate cutter or router, what it would see in cutting .125 of
plywood is a smaller tug than a Trump masturbation session. It shouldnt be the issue.
I cant count the number of times over the years the users trouble turned out to be the
connection from stepper to pulley or screw. The result is very like what your gear looks like,
but then , many such problems lead to a similar gear result.

    Another important test is a circle, is it round? Roundness of a circle indicates no backlash,
if its oval, theres a problem. Try something like

M3
G1Z.25 F10
G1X2.5
G1Z-.1
G3R5 X-2.5Y0
G3R5 X2.5Y0
M5
M30

  Do that after zeroing in the center of your table. The G3'3 will cut a circle
of a radius of 5" if you are zeroed in the center of your table. The resultant
circle cut tells you a lot about your machine. If round, great, if it leans left
in an ellipsoid, backlash , where the lean is will show the guilty axis,
how deep the Z is when problems start and where the problems start
tell alot about whats going on. Try it and post the result. Just change Z-.1 to
any depth to see reactions at various stress levels.


Art