Issues with tool paths - Fusion 360 to Centroid totally diffrent. <solved>

[tblough]

Post some photos of your machine at the home position, of the screen showing the machine coordinates (should be 0), and the screen showing your WCS position.

[cncsnw]

Did you choose to home both axes in their minus directions, or did it just somehow happen that way?

It is most common on a lathe to home both axes in the plus direction. In some rare situations (e.g. to avoid a tailstock which might or might not be advanced) some people will home Z minus, but only after homing X plus to ensure any tooling is clear of the part.

[tomb]

I did change the automatic homing direction to negative, if i left it positive, it homes towards the chuck?

Homes towards chuck -

Homes away from the chuck (Also the settings i'm on now with the problems i'm having)

I would like to set the machine to industry standard with homing in the plus direction (Without it homing towards the chuck!), the directions seem flipped. Doing that would also seem to solve my Fusion 360 issue as it wants to work in that orientation as well.

Not sure how to do that.

This might be a stupid question but have i wired my stepper motors in reverse?

[vw_chuck]

The red line that goes through your part is because that is the tool change position (G28) You need to set the G28 position behind the part for the longest tool so you don't crash into the part.
The one bad thing about Centroid is that it moves the X and Z axis at the simultaneously to get to the tool change position. If we could tell it to move X and then Z the chances of crashing would be eliminated. Don't feel bad Centroid it took many complaints and crashes for the the Fusion 360 guys to finally update the PP for this.

[cncsnw]

You need to reverse both axes, so that Z+ is away from the chuck, and X+ is away from spindle centerline.

I would do that on the Machine Configuration -> Motor Parameters table (F1/Setup -> F3/Config -> "137" -> F2/Machine -> F2/Motor) by toggling the "Direction Reverse" column from No to Yes. However, I am told that is not "user friendly", so there is probably a selection somewhere in the Acorn Wizard that does the same thing.

With the home position at the Z- and X- limits, if Intercon were to post codes that move X before Z, it would still crash. It would just crash closer to the chuck.

[tomb]

Progress! Thank you for your help guys, nearly there, i think there is just one problem left and i might see some chips.

You were right the axis needed flipping, i found the reverse axis's in the wizard.

Z- is now towards the chuck and X- moves towards center line.

To follow on from the line passing through the part, you were 100% right about G28, so i set that up and the graph looks correct but i get a error message saying X's axis is being exceeded, it's only set to 5mm in the return window?

Any ideas? i feel like i'm close now.

[cncsnw]

Since machine zero (machine home) is at the X+ and Z+ limits of travel, your G28 coordinates must be negative, or zero.

The G28 coordinates are the distance from machine zero (not from part zero).

[tomb]

Thank you, changed that and the error has gone.

One last problem and i think i'm there. I'm setting my part X and Z to 0 by touching off as instructed in the "Part" menu (See photo 1 and photo 2) but the program is treating this as the center of the part, so it is starting twice as far away from the part and when it thinks it is reaches the center of the part it is actually just touching it. I've attached photos of what i am doing, maybe you can see what I've done wrong.

(I'm using tool 1, offset is 0 as shown in photo 3)
(Photo 5 is the program stopped right after is starts to show where it's starting from)
(Photo 7 is what the WCS is reading after stopping it)

[ghack]

I have yet to run centroid lathe but have run several others, when you touch off in X you need to enter the part diameter not zero in the part touch off.
AND PLEASE SET YOUR FEEDS EXTREMELY SLOW as in barely moving until you get the hang of it.

[tomb]

Thanks for that! i'll try that now and hopefully we'll have some chips

It's not come out of slow mode yet