Router Forums banner
1 - 5 of 5 Posts

·
Registered
Joined
·
2 Posts
Discussion Starter · #1 ·
So I was cutting a part on the CNC, the first 2 operations used the same tool so the machine went through no problem until the end of the second operation where for no apparent reason it plunged about 1/8" into the vacuum table then tried to pull out and pulled the MDF off of the table. I hit the emergency stop and checked my CAM program simulation and it doesn't show anything like that happening.

I haven't had time to check the G-Code but I am planning on looking at it tomorrow.

Anyone encountered this?

My setup:

Laguna SmartShop II 48" x 96"
CAM: Fusion 360
 

·
Registered
Joined
·
372 Posts
A few things to check (besides the g-code):

When you save your g-code is the "use G28" checked? Is G28 defined?

Where is Z=0, top of material or top of spiilboard? Same for both tool paths? Were both toolpaths part of same CAM "setup" in Fusion 360?

Does it look like bit may have slipped in collet?

Are you a regular user of Fusion 360 or was this a relatively new experience?

Was there anything else running on you cnc control computer at the time (software update, antivirus, etc.).
 

·
Registered
Joined
·
2 Posts
Discussion Starter · #3 ·
A few things to check (besides the g-code):

When you save your g-code is the "use G28" checked? Is G28 defined?

Where is Z=0, top of material or top of spiilboard? Same for both tool paths? Were both toolpaths part of same CAM "setup" in Fusion 360?

Does it look like bit may have slipped in collet?

Are you a regular user of Fusion 360 or was this a relatively new experience?

Was there anything else running on you cnc control computer at the time (software update, antivirus, etc.).
Thanks for the reply BalloonEngineer. I don't see G28 as an option, and looking at the code it isn't used. Should it be in the Post?

Z=0 is the bottom of the stock, the program is set to leave 0.10" of stock at the bottom. Yesterday I didn't have a spoilboard (doh!) but this morning I put a spoilboard down and used "ZSpoil" offset in my controller.

No slipped collet.

It did it in the first operation when I ran it this morning.

I have cut a few things with fusion, it has dragged the top of a piece once but that was it. It seems to be going to the program's Z0 not the machine's Z0.

Full disclosure I am by no means experienced. I've just read a whole hell of a lot and played with the program for a long time before getting my router, so please forgive me if this is an amateurish issue.


Here's how the g code reads at the end of the operation:

N15805 G00 Z1.35
N15807 M05
N15808 G53
N15809 G00 Z0.

(next lines of code are the next operation)

I am considering using my NC editor and replacing line 15809 with G28.

Your thoughts would be much appreciated.

-Ronnie
 

·
Registered
Mike
Joined
·
3,843 Posts
One thing I notice N15808 G53 does not contain coordinates so there should not be anything prcessed on this line.

N15809 G00 Z0 tells it to go to Z0 so if you are zeroed on your spoil board it should move the bit down and just touch the spoil board, you say it went 1/8" into your vacuum table. You say the bit did not slip so there might be another problem that made you loose steps. If you top out on the Z axis you could loose steps and that could cause the machine to think the Z axis is located higher than it really is, This is a common problem on machines with a short Z travel but could happen on other machines.

Another thought, and I kind of think this may be your problem because you say it happened again at a different location when cutting the same thing again, would be the Z axis screw is loose where it attaches to the stepper motor allowing it to loose steps or is moving up and down. If it has set screws make sure there is not a locking set screw in the hole when you tighten it. If it does have an extra set screw to lock it on the shaft you need to remove it to tighten the actual clamping set screw then replace the 2nd set screw to keep the first one from working loose. Might be in a different part of the Z axis mount but I do think it is a mechanical problem.
 
  • Like
Reactions: difalkner

·
Registered
Joined
·
1,216 Posts
G53 puts the machine into absolute coordinate mode, and everything after that command might be offset from where the previous commands were moving the machine. The following G00 Z0 then could be what sent your bit into the spoil board.
 
1 - 5 of 5 Posts
Top