Acorn Lathe Intercon help needed

[slodat]

Hello. I have a gang tool lathe (link to build thread is in my signature). I've attached a fresh report and the intercon file in question.

I'm trying to sort out how to manage moving the gang tooling around between operations, so I don't crash a tool. T0101 is my longest tool. I'm wanting to have it go to +1 Z between moves, then move to the next tool's X +.6 (.5" diameter stock), and then proceed to next operation..

For some reason on the turning operation the control just keeps going +Z for each pass. If I don't stop, it will go to the Z+ limit.

I think I've done something dumb in the intercon, but I don't know what.

I appreciate any help!

Thank you.

[slodat]

Can someone give me an example or an approach of how to make the Z+ moves, then X moves to avoid a tool -> work piece collision on a gang tool lathe? The Rapid move in intercon moves X and Z at the same time. I’m thinking it best to move straight in Z+ to a safe Z with little or no X movement.

I’ve searched and read all I can find and it all says you have to manage these moves yourself. I haven’t found examples of how to do it.

Thank you!!

[suntravel]

You can use Pre/Post Cycle Pos. like shown here for retract 1" in Z

related reading and video:

https://centroidcncforum.com/viewtopic. ... ing#p64821

Uwe

[slodat]

When I tried using the post position it moved in X to X0, which can easily crash. Need to only move in Z. Is there a way to have it only move Z?

Also any idea why it’s moving in Z+ during the turning move I described in my first post?

[suntravel]

After T0101 all tools are going to x0.6 and Z1 now.

Uwe

[slodat]

Uwe - thank you for working with me on this. Unfortunately the intercon file you posted doesn't work for my situation. This is a photo of my tooling block's current configuration:

The long boring bar on the far side of the tooling block is T0101. The pre/post moves go in X and Z at the same time. This will crash the tool on the work piece every time. I'm trying to understand how to move out to a safe Z+ "retract" distance, then move over in X, for each tool.

[cncsnw]

You have to choose an appropriate X value for each pre/post cycle position.

For example, in your N7 OD Turning cycle with T1, retracting to X0.52 Z1.0 should work.

In some situations, you may also need to insert a Rapid (Line, in Rapid mode) move in between canned cycles, to put either the previous tool or the next tool where you need it.

For example, when you are done with T1 and want to move to the threading tool, you might insert a Rapid that moves T1 to X-2.0 Z1.0, so that the boring bar is safety beyond the stock, before you switch to the T4 offsets and head for the start of the Thread operation.

[suntravel]

In the Intercon setup
Suppress G28 for ToolChange = Yes

And config Parameter
Parameter 6 = 1

I added two rapid moves in the file.
The first moves T0101 behind the part before the next shorter tool goes to start position.

Uwe

[suntravel]

Another way is to turn the boring bar and threading tool 180° and let them work on the rear -X side...

Uwe

[slodat]

I'm finally back on the lathe. I had a motion issue that I think is solved. I won't know until I run a few programs. What I have attempted to do in Intercon is create a program to turn what is essentially a bolt, thread it, then part off. I upgraded to CNC12 v5rc4. It's got some nice new features. What I'm running into is when I go to graph the part, I get a Z axis feedrate exceeeded in block N5 which is the threading block. When I post the code and graph it says it is in line 82:

Code: Select all

G76 X0.1894 Z-0.5 R0.0 P0.0277 Q0.005 F0.05

This is the whole thread cycle:

Code: Select all

; --- Thread Cycle ---
N0005 T0400 ;Boring Bar Threadin
  M9
  G97 S600.0 M3
  G4 P3.0
  X0.6 Z1.0 T0404
  X0.4449 Z0.0 
  G76 P010000 Q0.001 R0.003
  G76 X0.1894 Z-0.5 R0.0 P0.0277 Q0.005 F0.05
  X0.6 Z1.0 
  M5
  G50 S2000 ; max CSS spindle speed 

I'll admit, I'm struggling with Intercon in general. I know it's very capable and once I get the basics of how it works I'll be in good shape. Getting there is kicking my butt right now.

As I mentioned in the first post of the thread, there's a lathe build thread link in my signature. I appreciate any help or advice. I'm betting it's something simple that I'm not seeing.

edited to add: I get the same Z axis feedrate exceeded with Uwe's intercon file above..

edited again to add; I'm struggling to see where the feedrate for the G76 would even come from?