Exceeding travel

[suntravel]

Value tool offset 0909 23.6309 plus G0 X1.175 Z0.1969 T0909 is more than x+24.1759 shown at home position.

Uwe

Im trying to wrap my head around what you're saying but I don't get it. Gone over it and over it trying to make sense of it. What is the 1.175 in X you're adding to the tool offset? I could see if you're adding the stock radius but that's not it because its .375 Di stock so what is the 1.175?. AND why are you even mentioning the Z value? How does that even come into play? Can you please explain?

On the pic with the home notice, machine ist at x 24.1759
If the tool offset is 23.6309 and you try to go 1.175 further like in line 82 , this would be behind 24.1759 and if you want to go behind homing position travel ex error comes I suppose.

Right now I am only using centroid for a mill, converting my lathe to centroid religion comes next

Uwe

[BillB]

1.175 is the X diameter on line 82 of your program, where you said the error was reported.

That line of the program turns on offsets (T0909) and tries to move the tool tip to X1.175 Z0.1969.

Try activating the offsets in MDI ("T0909"), then jogging the axes until the X axis on the DRO reads 1.175.

If you are trying to part off 0.375" stock, maybe you could start with the cutoff tool at a closer clearance than 1.175".

So this is a clearance move causing the issue. NOW I GET IT ; ) NOW I SEE how I could resolve it.
I come away from this info with a few things in mind. To avoid this I could do one of the following?
As you said less clearance in X in my programming, which Ive changed "reluctantly" since Im a lathe newbie: { Strange because the current value is just default.
Shorten my tool length.
OR
I could move tool 9 down closer to the inside of the gangplank?
This also means the distance my tool #9 is sitting right now is basically borderline 'way to far out on the table" because EVERY program Ive tried to run since getting set up has failed with exceeding travel limits on tool.

Well that sucks!

cncsnw
When you say "activating offsets" Isn't this the same thing as changing the tool in MDI since this tool # and its offset are the same for this tool? However, the tool # and offset # can be different? Correct? thought I seen that somewhere?

[BillB]

Value tool offset 0909 23.6309 plus G0 X1.175 Z0.1969 T0909 is more than x+24.1759 shown at home position.

Uwe

Im trying to wrap my head around what you're saying but I don't get it. Gone over it and over it trying to make sense of it. What is the 1.175 in X you're adding to the tool offset? I could see if you're adding the stock radius but that's not it because its .375 Di stock so what is the 1.175?. AND why are you even mentioning the Z value? How does that even come into play? Can you please explain?

On the pic with the home notice, machine ist at x 24.1759
If the tool offset is 23.6309 and you try to go 1.175 further like in line 82 , this would be behind 24.1759 and if you want to go behind homing position travel ex error comes I suppose.

NOW I get it, THANK YOU! What a journey this has been, Gang tool lathe is defiantly harder than learning the mill.

Right now I am only using centroid for a mill, converting my lathe to centroid religion comes next

Uwe

[BillB]

Not out of the woods yet boys.
So I was able to resolve the issue with the travel in X and successfully run the grove and part off tool path for the first time without any exceed travel error. SO that's good, I changed the clearance diameter in Fusion to where it was at about .58 something to 1/2 that and that fixed the issue. Thank you guys for helping to understand what was going on, now I know what to look for and how to resolve it from here on out "hopefully"

BUT did I say Im not out of the woods yet? SO now the last thing to resolve is a tool orientation issue. What is happing now is the tool is approaching the stock and going beyond the chuck's center to the bottom-most side of the cut then retracing in X-. So basically the tool path and movement are inverted, thus the tool movement is inverted. This is all due to Fusion and how it is currently handling a gang tool, tooling set up, OR should I say the "lack of" how handels a tool coming in from the top of the stock side. It doesn't! Fusion currently does not support tooling that comes in from the top approach. I have been getting to the bottom of this with the Fusion support forum and going over the details with one of the AD techs on it. He has told me that for any top side tooling to just define the tools as if they are coming in from the bottom side like a standard lathe tool set up. Explaining that in the post things will be adjusted and the cut will work correctly.

As per his input, i have changed the tool approach from the bottom as you see in the screenshot. IF and when I define the tool with a top approach it will not generate a tool path and the tool and holder is displayed in RED as seen in the other screenshot.

SO question is, IS this a Fusion thing that needs to get worked out in the post OR a CNC12 setting that needs to get changed? OR to fix this would it require a custom post? AND WHO would do that? Would Centroid?

I am told by the AD tech that resolving this and supporting tool orientation is a way off from being implemented.
Here is my post if you want to read threw it.
https://forums.autodesk.com/t5/fusion-3 ... 01#M115999

Here's a video to clarify.
Video coming in a bit

[suntravel]

for lathe parts without 3 axis and driven tools, it is way faster to use Intercon than messing around with fusion...

Uwe

[tblough]

If you can program it correctly in Intercon, then it is a Fusion issue. It might tequire s custom Fusion post.

[suntravel]

IMHO you have to learn to walk before you run....

Read the manual, make simple programs with Notepad++

Make simple programs with Intercon, read and understand the g-code coming out of Intercon

If you still want to use CAM like fusion after this, you will have the knowledge to make external PPs work with Acorn.

Uwe

[cncsnw]

If a tool cuts from the X-minus side of the spindle (whichever side that may be), then cuts with that tool need to be programmed with negative X diameter values.

That is true in Intercon, and it is true in G codes.

To get correct results with any given CAD/CAM system, the post-processor would need to generate negative X values whenever you use a back-side tool.

[BillB]

Guys here is the video of the inverted cutting motions.

[BillB]

If a tool cuts from the X-minus side of the spindle (whichever side that may be), then cuts with that tool need to be programmed with negative X diameter values.

That is true in Intercon, and it is true in G codes.

To get correct results with any given CAD/CAM system, the post-processor would need to generate negative X values whenever you use a back-side tool.

It would be really helpful if you could give me some detail on how to approach programming the backside tool/s with negative values? Would be really appreciated.