TURNING - Finish OD and face

[Ryan_Fab]

Good Morning,

I'm new to the turning environment and I've ran into an issue.

I would like to finish externally and then run down over a small portion of the front vertical face with the same command. Is this possible? 

My file is attached. Any help would be greatly appreciated

Cheers 

[christopher.cooperVHK2N · Accepted solution]

@Ryan_Fab I don't believe this can be achieved using the body but you can do this by driving the toolpath through a created contour. The contour is created in the Design workspace and selected in the operation settings.
A small horizontal line is needed for the lead out after the desired X point is achieved.

[engineguy · Accepted solution]

@Ryan_Fab 

If this is anything like what you need then try the attached file

[Ryan_Fab]

Both are great, thanks guys. Im using the sketch one in this instance as it allows me travel back to front.

I appreciate the help

[Anonymous]

Here is your back to front pass using model 😁

l 

[Ryan_Fab]

Brilliant!.... but what did you change!? Im still missing something because I cant replicate it 😫

[Anonymous]

If you unselect radial extension in linking tab, tool makes facing move.

[Ryan_Fab]

Brilliant, makes sense and yet the only thing I hadn’t tried 🤣

[christopher.cooperVHK2N]

@Anonymous Well that saves me sometime also, thanks.

Seems strange that you have to uncheck the box to extend the toolpath radially.

[Anonymous]

This is another example of poorly managed user interface, function that serves purpose in cutting front to back is contradicting factor in cutting back to front.

Looking at definition of the function, it extends pass to stock diameter in front to back cut and because of its intended direction of extension, if enabled, it prevents tool from going in opposite direction to face off part when cutting from back to front even though all other settings are correct.

In practical terms this has no useful function at all and here is why. If I am cutting 1." diameter part out of 3." diameter stock, I need to extend rough cuts in Z axis to accommodate cut off tool but I don't need to follow up with finish pass over entire surface, I only need to finish 1." diameter and extend pass past the back edge in Z axis.

From there I need to retract tool in X axis and pull away in rapid mode, what purpose is there to waste time finishing rough cut to outer edge of stock?

If using G70 cycle to follow after G71/G72/G73 cycles, tool will follow entire path of roughing cycles, adding cycle time and needlessly inflicting more ware on cutting edge.

Using function in Fusion to mimic that behavior is pointless and undesirable.

In hand coding, use of G70 cycle is quick way to apply finish pass after roughing, I use it mostly for cutting jaws with same tool.

If the function remains part of the finishing strategy, it needs to confirm to other settings, disable it when back to front cutting is selected by user.  

[akash.kamoolkar]

@Anonymous i've made a ticket to hide the radial extension parameter for cases where it does not apply.

Thanks,

Akash Kamoolkar

[gvisserVMT]

I need this function, but it doesn't exist anymore.

Can someone help me!

[christopher.cooperVHK2N]

@gvisserVMT It has been removed in certain cases for the March release.

@akash.kamoolkar Is the new workflow for the user to use the 'Linear Lead out Length' to control the face portion when machining back to front?

[gvisserVMT]

I gave the linear lead out angle a 315 degrees angle and a linear lead-out length of 18 mm. Now it works!

[christopher.cooperVHK2N]

@gvisserVMT I had set the angle to 0 to make it go down the face and increased the lead out length.

Need to make sure the lead out feedrate is the same as the cutting feed.

Still not 100% this is the correct solution though so would welcome other opinions.

[akash.kamoolkar]

@christopher.cooperVHK2N @gvisserVMT The "radial extension" parameter only applies to when the finishing operation ends in a stock wall and you want to keep machining up the wall up to the outer radius. This is only relevant for certain combinations of the insert orientation and direction of machining. What are you trying to do here @gvisserVMT maybe you can attach a file?

Thanks,

[engineguy]

Is this what is required ?? Back to Front Profile Finish with end Face ?? See Screencast.

Screencast link :- https://autode.sk/3iItq4n

[gvisserVMT]

That's correct.

The only problem now is that the product will become to short. I can't program a radius compensation or extension.

[gvisserVMT]

This is an example. The toolpath is going as wished, but the total length of the product will become to short. What can I do about that?

[christopher.cooperVHK2N]

@gvisserVMT I offset the front slightly to allow the tool to reach Z0 and it posts correctly for me.

So it looks like Lead in is not the way to achieve this. Rather a combination of 'Front' and 'Inner Radius' offset.