My new Shapeoko 3 is it just me?

[Rocket]

Art,

I have tried the attached file many times...in Universal G code sender
and in Carbide Motion.

Each time the same thing, as the spindle starts to move it drops down
a few MM's.

They will come to take me away soon....

Lost..........

[Rocket]

I just thought of something, none of the above problems occurred
when I ran a program that was a demo from Cut 2D Desktop.

The tool-paths were created in C2D, then saved, and run with Universal G-code
Sender.

Clean cuts.........no drag line from first position to start of cutting...

Does that info help any???

R

[Rocket]

Art,

Here is the small sample file from Cut 2d Desktop,

No drag works well....no problems

[ArtF]

Rocket:

  Put the G20 at the very top, above everything... other than that it shoudl run fine.

Art

[Rocket]

Art...Art...ART.....

I think you are going to be very proud of me,,,,,,(I hope) but I could be wrong.....

Every gear I made in Gearotic for the past two weeks has done that
drop down from the start and made a cut on the way to the center hole...not good...

So after many hours of watching this over and over in a simulator, I came to the
conclusion the it was the first line under M3 S1750: that reads:
G1 Z-0.050  F20.00  (See attached .tap straight from Gearotic).

All I did was add G20 and change that line to read: G1 Z0.25  F20.00
See photo of my best gear yet....( I am so excited....!!!)

Without your help...........I would be in big trouble....

Thanks................rocket

[ArtF]

Rocket:

When you execute a G1 Z0.25  F20.00 , the tool should go up, not down.
For you to cut the gear, it must have gone down. Which mean when you execute Gearotics normal file ,
its line of  G1 Z0.25  F20.00 at the beginning , which should have made it go up, actually made it go down..

  I suggest you make sure, does G1Z1 make the tool go up or down.. Try a file with just the following in it,

G20
G1Z.25F20

Does this file make the tool go up, or down?

Art

[Rocket]

Yes....it goes up.

But, if you look at the attachment here you will see that line says:

G1 Z-0.050  F20.00

That came straight from a Post from Gearotic, I did not change anything
in the original attachment 999straight from Gearotic.tap.

I discovered I had to change it to G1 Z0.25  F20.00.

Why is the post from Gearotic make the spindle go down?  See attached .tap from Gearotic.

I am confused, I think...

I would be happy to speak with you on the phone ( I could call you)
or use regular email so we can communicate easier.

My personal email: rocket2004@comcast.net

[ArtF]

Rocket:

  Theres nothing wrong with the file, you just need a G20 at the very very top.

  This is why I say until you understand what the commands are, its hard to understand whats
happening.. but the position of the G20 means everything... Look at the comments following each line below,
Ill show you what happens the way you were doing it, and the way it needs to be done. Only the first few lines matter..
This is what you have, ( and Ill remove the comments.. anything in ( )'s are a just comments and can be removed..

  This is what gearotic is giving you..

G0 X3.445  Y3.307  Z0.250  A0.000  //move to center of gear at 3.445" in X, and 3.307" in Y , and 1/4 inch up..
M5          //turn off spindle
M6 T5      //change tool
M3 S1750  //turn on spindle at 1750 rpm
G1 Z-0.050  F20.00    //move down to -.05
G1 X3.441  Y3.307  F50.00  //start cutting..,

  This code is fine and will work on an imperial machine. BUT, your machine is metric, so you
need to add a G20 to make it work. You keep adding G20 after the first line, that wont work. Here's why
... Your machine starts up in metric, and doesn't switch till it sees a G20.. so follow this... the first move,
your machine thinks is in millimeters..

G0 X3.445  Y3.307  Z0.250  A0.000  //move to X3.445MM, Y3.307MM and .25mm up..

G20 // your then adding a command to switch to inches.. so your now at x= .135", Y= .13 ", not in the
          center of the gear to start at all, but thats beacuse the G20 wasnt executed before the move to center
          above..

M5
M6 T5
M3 S1750
G1 Z-0.050  F20.00  //move DOWN, because it thinks its at 3.445",3.307" , but it isnt, its
at 3.445mm , 3.307mm because the first move happened while you were still in metric.

G1 X3.441  Y3.307  F50.00  //now its down and moves to center cutting a line in the gear..
G1 X3.438  Y3.308 
G1 X3.433  Y3.308 

  So just put a g20 at the TOP of this file, no other editing.. it will work fine. In Gearotic ,
you can set a setting called Prologue, set just "G20" in there and Gearotic will add the
G20 for you as you create the file.

  You can always reach me at support@gearotic.com, I don't do phone calls, but Im always
reachable..

Art

[Rocket]

Okay..........I have tried all things you said in your last post about
10 times....each time if the only thing I edit is inserting G20 at the top
it continues to drag a cut through material before it gets to center hole.

The only way I can stop that from happening is to:

1.  Insert G20 right above the M5 command:
 
M5
G20

Then I must take the line that says: G1 Z-0.050  F20.00
and remove the minus (-) right after the Z.

So the new line there reads:  G1 Z0.050 F20.00

When I do those two edits the spindle travels from point of
origin to point of drilling center hole with no up or down movement.

Which makes me believe that the - (minus) sign in front of Z was
making the spindle go down before it reaches the center drill hole.

Am I nuts.....?????

rocket

[ArtF]

Well, if it works for your machine, then keep doing it, but as I read it , there is no drop to start the cut
if you change that Z to + instead of minus. Does it actually cut the gear after you edit, or just trace the gear in the air? This isnt so much about the Gcode, but the way your machine reacts to it, have you asked the maker where the G20 should be, or if there is some way to permanently set it to imperial?

  Personally, I think what you need to do is write several programs of your own, until you
understand why its doing whatever its doing. All I can really say from here, is the file your
showing from gearotic has been cut by thousands of machines with no line...

For the record though , here are the first lines of Gearotics file, and what they do,
you should be able to simply see what line isnt doing as it should.

( No Prolog Set )( GCode Objects Begin. )        //comment, does nothing
( Object Ratchet Begins )                        //comment, does nothing
G0 X3.445  Y3.307  Z0.250  A0.000              //Move to center of gear and UP to .25"
(  Shaft Hole path - Inside Profile )                    //comment, does nothing
( Tool --: EndmillInch-E-R0.13-T0.0-F0.0 posted as T5 ) //comment, does nothing
M5                        //spindle off
M6 T5                        // tool change, should do nothing on your machine, remove it if you like
M3 S1750                    //spindle on, if your spindle is manual, remove it if you like.
G1 Z-0.050  F20.00                // move DOWN, but ..as of line 3 above, we're not at the
G1 X3.441  Y3.307  F50.00        //start of the gear, we're in the middle of it.

  If you are dragging aline through the gear, then the line

G0 X3.445  Y3.307  Z0.250  A0.000

is being ignored. This line places you in the middle of your gear BEFORE dropping.
Why its not in center, I dont know, mine would be. Your gonna need to ask someone
familiar with your controller why on earth its ignoring the first line of motion.
Changing the line from - to + will stop all cutting near as I can see..


    Now its possible your table isnt flat, or some other issue exists.. all I know
for sure is that these three lines tell it NOT to drop until its in position..

G20
G0 X3.445  Y3.307  Z0.250  A0.000 
G1 Z-0.050  F20.00 

  Make a file with just those three lines, what does it do when run? Does it move to
center of gear while going up? Or does it cut the line to center? Just copy those three
lines into a file , zero as normal, run it, and let me know what it does. That alone should tell us
how to proceed.  Perhaps on the first lien change Z0.25 to Z1 so you can really see it raise..



Art

[Ya-Nvr-No]

This is where Art is telling you to place the Code
you seem to not be seeing the first move that puts you in position for the first feed move down.

( No Prolog Set )( GCode Objects Begin. )
( Object Ratchet Begins )
G20 (Imperial Mode)
G0 X3.445  Y3.307  Z0.250  A0.000  (this is a rapid move to the center 1/4" above part face)
(  Shaft Hole path - Inside Profile )
( Tool --: EndmillInch-E-R0.13-T0.0-F0.0 posted as T5 )
M5
M6 T5
M3 S1750
G1 Z-0.050  F20.00
G1 X3.441  Y3.307  F50.00  
G1 X3.438  Y3.308  

[Rocket]

This is where Art is telling you to place the Code
you seem to not be seeing the first move that puts you in position for the first feed move down.

( No Prolog Set )( GCode Objects Begin. )
( Object Ratchet Begins )
G20 (Imperial Mode)
G0 X3.445  Y3.307  Z0.250  A0.000  (this is a rapid move to the center 1/4" above part face)
(  Shaft Hole path - Inside Profile )
( Tool --: EndmillInch-E-R0.13-T0.0-F0.0 posted as T5 )
M5
M6 T5
M3 S1750
G1 Z-0.050  F20.00
G1 X3.441  Y3.307  F50.00  
G1 X3.438  Y3.308  

I have done that about 15 times and it does not work.
For some reason it is ignoring the line: G0 X3.445  Y3.307  Z0.250  A0.000

[Ya-Nvr-No]

what does not make sense is it works by the time it sees a G1 Feed move.  ???

Might try rearranging the order

G20 (Imperial Mode)
M5
M6 T5
M3 S1750
G0 X3.445  Y3.307  Z0.250  A0.000
G1 Z-0.050  F20.00

if the above code does not work I would find a new home for that machine ASAP
and I would suspect that controller has other issues.
You don't get any more basic than what Art has provided.

Edit addition: In over 40 years I've never seen a controller do that.

[Joakim]

Shapeoko is based on GRBL motion controller and as I understand it, GRBL only works with 3 axis (X, Y and Z).

Code: Select all

G0 X3.445  Y3.307  Z0.250  A0.000

Could be ignored because the A0.000 coordinate is not supported.
I would try to delete the A0.000 part of G0 and follow Arts suggestions.

Just a thought.

[Rocket]

Art

I in no way would question anything you say about any of this,
I would very happy if I know 2% of what you know in the next few years....

I just sent this same .tap file to Carbide 3 support team and asked them why?????

I just made this gear (.jpg pic attached)
with that same file, All I did was remove the - (minus sign) from the Z line.

The attached file is the file I used to  makee this gear with.....
I have no idea.....maybe Carbide 3 (Shapeoko guys) can answer us????

I am smart enough to know when I am dealing with smart people!

Thank you..................I know that I have been a pain in the ass........

r