What's new
What's new

Starting mid-program crash

Barry680

Plastic
Joined
Sep 21, 2017
Is there anything to watch out for when starting a program -not- at the beginning? using G90 absolute programming..

The actual program ran fine from start to finish but threw up a burr on the chamfer pass... I then started mid-program from the contour pass (N5640) to clean up the burr and the spindle went, or at least tried, to Z-7.ish destroying all you can imagine.

If anyone wants to see the code....

It's not a one off error, I ran both ways again with the same results, start from beginning and it's fine.. from N5640 and it tries to crash.
Maybe it's just the machine, it's new but was recently updated to fix other known bugs.
I just want to know if I'm to blame before I go pointing fingers.
 

mutiny

Cast Iron
Joined
Jan 27, 2019
Location
Raleigh
My thought (not an expert): I don't see a G43 anywhere, which would normally be setting the tool length offset. It's possible that your control is configured to automatically set the offset at a tool call (Tn M6), but starting at the line you did skips that.

If you insert a T33 M6 (I think the chamfer was 33) at the start of that section, is the result what you expect?
 

Barry680

Plastic
Joined
Sep 21, 2017
I'm doing tool diameter offsets in CAM, not at the control.

It is using the same tool as the face, a 3/8 end mill. The stock is 0.097" (Y) thick so no need for a large tool.

When I get back I'll see if adding/starting from a tool call makes the difference.
The program always goes back to the first tool at the end of the program, it does look back and tool change to the correct tool before the crash though so maybe it won't help... hmmm...
 

Freedommachine

Hot Rolled
Joined
May 13, 2020
My thought (not an expert): I don't see a G43 anywhere, which would normally be setting the tool length offset. It's possible that your control is configured to automatically set the offset at a tool call (Tn M6), but starting at the line you did skips that.

If you insert a T33 M6 (I think the chamfer was 33) at the start of that section, is the result what you expect?

I agree with this^^.

Did you hit reset before your attempted restart? If so, that may have wiped out your tool length offset.

At N5645 Try this G43 H13 Z.6;
The tool call up that mutiny stated would probably work as well but it might send the machine to the tool change position first. (Depends on the machine)

Edit: You might also need to add a G54 to whatever line you're starting on. Most machines default to G54 but might be different in your case.

Turn rapid down and single block on. Set feed pot to 0% and hit cycle start. Now turn feed pot up to allow the machine to move. If you want to stop it; turn feed pot back to zero. Watch "distance to go" screen.

Always do this when you aren't 100% sure. It is a safe way to creep into something without crashing. ;)
 

nscele

Aluminum
Joined
May 30, 2007
Location
Australia Qld
What machine and what control?
none of the tool changes are using tool length comp - G43 H** , on my one machine this is fine, Siemens 828d but it has a proper restart procedure.
 

Barry680

Plastic
Joined
Sep 21, 2017
ProtoTrak TMC7 with RMX control. I bought it as a first CNC machine to learn on...

The conversational programming is extremely limiting and likes to break tools so I started learning CAD/CAM.

As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion.
 

Dan from Oakland

Titanium
Joined
Sep 15, 2005
Location
Oakland, CA
"As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion."

That's like getting on a busy freeway and closing your eyes on the on ramp and hoping for the best.

You need to spend time understanding how your control responds to program code regardless of the format. If you are running G code- the same applies- take time to understand what its telling the machine to do. You can always ask questions here when you need help, but you have to do the basic ground work.
Lots of u-tube video out there- start with understanding what a "safe start block" is.
 

barbter

Banned
Joined
Oct 27, 2007
Location
UK
ProtoTrak TMC7 with RMX control. I bought it as a first CNC machine to learn on...

The conversational programming is extremely limiting and likes to break tools so I started learning CAD/CAM.

As far as what the control requires with G code, I have no idea, there really isn't any info in the manual about it, I'm simply relying on the post within Fusion.

I would contact SWI and ask the questions - a demo prog with a couple of toolchanges too.
On Fanucs you'd be having cancel codes at the start of the tool to clear drill cycles etc - this may need them???
 

mTeryk

Hot Rolled
Joined
Jul 4, 2010
Location
corvallis,or
On line N0030 you call G54 to specify your work offset. When you hit reset it likely cancels the G54 which you would have to reset if you want to restart mid-program.
 

Sandoz

Plastic
Joined
Aug 17, 2021
As mTeryk said it may be that when you skip over workpiece zero (N5465 G54), the control might use wrong zeropoint.
You can check if this is the problem by adding another G54 over the line where you want to skip and skip to that line instead. Edit: Or note where the tool is, skip to another line after N5465,push reset and without blank and with feeds at zero of coarse try it again. You should see a ridicilous minus Z movement to come.
 








 
Top