What's new
What's new

Mill losing part location on next tool/op

Radioactiv

Plastic
Joined
Sep 22, 2017
So next in my adventures of buying a used VMC as my first mill. I'm posting from Fusion 360 to a Sharp SV2412 w/ OI-MC . The first operation is perfect, done 2 separate ones on 2 parts. One was a adaptive 1/2" EM cut.

As soon as the machine changes tools the XYZ are not even close to lining up with the part on the 2nd tool. I haven't tried using the same tool on separate ops yet but thats tomorrow. I'm hoping its something simple that I'm missing and not something serious like the encoder going funky.


Tool 1 start location N60 G00 X7.299 Y-0.475

Tool 2 start location N170 G00 X6.3092 Y-0.4108
 
Look at the G-code. Does the location in the G-code for tool 2 agree with where it goes? Is there G54, G55 in the G-code. Those are work offsets and you could have them set differently.
 
Look at the G-code. Does the location in the G-code for tool 2 agree with where it goes? Is there G54, G55 in the G-code. Those are work offsets and you could have them set differently.


The 2nd tool goes to G54 just as the 1st tool, so i dont think that would be the issue.

You need to post a copy of the code you are running.

Mill1 - Pastebin.com


There is the code, let me know if you see anything off but from what I can tell it seems fine. :willy_nilly:
 
So tool 2 is tool 3.

Where is the machine after it makes the tool change and the positioning move? Also wonder where it's sitting at the op stop just before the tool change.
 
Just thinking out loud, offset in the tooltable from the previous owner? Like angle drive usage?

Marko
 
Your code is fine. The machine is going where it's programmed to go.
Your tools are two different diameters so I would expect that if you're starting each tool a certain distance off the feature you're machining the start point would be different.
 
Code is good.

I'd start by checking tool offset locations. Make sure you didn't fat finger something during your set up.
 
I'll try to just get a video of the machine up some point today since its decently hard to explain. But it picks up the 2nd tool, Z goes up probably 12+ " above the part spindle turns on. X and Y seem to be at least 6" off the part.
 
I'll try to just get a video of the machine up some point today since its decently hard to explain. But it picks up the 2nd tool, Z goes up probably 12+ " above the part spindle turns on. X and Y seem to be at least 6" off the part.

Look at your tool offsets. Maybe there is a crazy offset that someone used to verify something...? (not looked at the code btw)
 
Try a G90 after the tool change. Maybe M06 calls a tool change macro that leaves it in incremental. You said X is about 6" off. Looking at your program, the last X and next X are about 6" apart.
 
I would go back and look at your CAM file. The code for T3 looks like it is programmed as the same tool diameter as T1. I can't imagine it runs fine if run by itself.
Also, your code is for T1 and T3 yet in your posts you refer to tool 2?
One last thing, your finish profile looks rather disjointed. Lots of small point-to-point moves and .010 arcs. Eventually T3 finishes at the same point as T1.
 
I would go back and look at your CAM file. The code for T3 looks like it is programmed as the same tool diameter as T1. I can't imagine it runs fine if run by itself.
Also, your code is for T1 and T3 yet in your posts you refer to tool 2?
One last thing, your finish profile looks rather disjointed. Lots of small point-to-point moves and .010 arcs. Eventually T3 finishes at the same point as T1.

I think he's calling it tool 2 as in "2nd tool in the program".

pmcode1.jpg

Looks about right to me.
 
Just went and reran it, made sure there were no other G54-G59s in. I was wrong about the X and Y, they seem pretty close to lining up. The Z is close to the machine home/ 0 position once it picks up the second tool in the op. (T3)


I almost feel like T1 is cutting relative to my G54 and T3 is trying to cut relative to the machine home.

I just made my first chips the other day so I could be messing up somewhere in my setup. First touched spindle to the vise and set that as relative Z then I went through and did that to all my tools. I then found G54 with spindle nose to part, and X Y with edge finder.

Am I missing something basic that would vary from tool to tool?

Ill attach a video and pictures to hope it clears things up.

Sharp SV2412 issue - Album on Imgur


Sharp SV2412 issue - YouTube
 
So next in my adventures of buying a used VMC as my first mill. I'm posting from Fusion 360 to a Sharp SV2412 w/ OI-MC . The first operation is perfect, done 2 separate ones on 2 parts. One was a adaptive 1/2" EM cut.

As soon as the machine changes tools the XYZ are not even close to lining up with the part on the 2nd tool. I haven't tried using the same tool on separate ops yet but thats tomorrow. I'm hoping its something simple that I'm missing and not something serious like the encoder going funky.


.
G43 H1 or what ever H needed is length comp
G41 D1 or what ever D needed is dia or radius comp.
G54 or G55 or whatever is work offset
G90 is absolute mode
G91 is incremental mode
......you need to find program check or monitor screen and see whats active. many machines
G41 D2 Y3.000
(COMMENT 1)
(COMMENT 2)
if you got 2 consecutive lines of non movement between G41 and G40 it messes up tool comp calculations. often see if its suppose to only move in X and you see Y changing slowly or tapering as tool comp tapers down to zero
 
Dodgin's post clears up some of my questions. Thanks.

Your setup procedure seems correct. I'm leaning towards what someone mentioned above: throw a G90 in after T3M6. There could be a G91 active from the toolchange macro.
 
Just went and reran it, made sure there were no other G54-G59s in. I was wrong about the X and Y, they seem pretty close to lining up. The Z is close to the machine home/ 0 position once it picks up the second tool in the op. (T3)


I almost feel like T1 is cutting relative to my G54 and T3 is trying to cut relative to the machine home.

I just made my first chips the other day so I could be messing up somewhere in my setup. First touched spindle to the vise and set that as relative Z then I went through and did that to all my tools. I then found G54 with spindle nose to part, and X Y with edge finder.

Am I missing something basic that would vary from tool to tool?

Ill attach a video and pictures to hope it clears things up.

Sharp SV2412 issue - Album on Imgur


Sharp SV2412 issue - YouTube


In your code it looks like you call a G90 at the end of the first operation.

In your video when you pan over to the screen it looks like G91 is active command.

Am I seeing that right?
 








 
Back
Top