Fusion360 - Profile Finish - Empty Toolpath with BACK TO FRONT

[Six1Seven1]

Hello.

Attempting to perform a very simple finishing op on a turned profile with a 35 Deg Diamond. 

Fusion throws an 'Empty Tool Path' error on the toolpath in question when the direction is 'BACK TO FRONT'.

I can remedy this by either allowing axial/radial grooving, or changing the direction.  I don't want to allow grooving. And I don't want the direction from FRONT TO BACK... It also using Rest Machining. 

@FusionDevs

This is a simple real-world scenario of a turning operation. If this is a challenge for Fusion to do, then perhaps it's not a suitable cam environment. Just my 2 cents. 

But I appreciate your insight. 

Attached.

[akash.kamoolkar]

@Six1Seven1 

Which specific area are you trying to machine with this operation? Area A won't be machined because there's nothing to machine there since you have rest machining turned on and your stock diameter is the same as the model diameter there. Area B won't be machined unless you turn radial grooving on which will allow the tool to enter that area.

Regards,

Akash Kamoolkar

[Six1Seven1]

Hi, thanks for you reply.

Indeed, good point about stock dia. However, moving the toolpath 'BACK POINT' towards Z0 where there is still in fact stock, results in the same error. See attached. 

There is .020" on the part OD from the roughing operation. The source for rest machining in the finish op is 'From Previous Operation'. 

There is .020" on the stock. No reason Fusion should be having trouble with this. 

[akash.kamoolkar]

@Six1Seven1 Unfortunately the way the software currently works the entirety of the part to the right of area A is considered a groove while machining from back to front, no matter where you put your limit and therefore ignored when grooving is set to "dont allow grooving". We're currently working on adding more flexibility to define individual grooves to suppress while machining to fix issues like this. For now there may be an alternative workflow to achieve what you are looking for. Is this the area you're trying to machine?

Regards,

Akash Kamoolkar

[Six1Seven1]

Unsure why this is an issue for Fusion. Its a simple turning toolpath in the reverse direction. Should be a simple fix.

To clarify for you, this is the area i'm trying to machine. The same as the roughing cycle... 

The groove is irrelevant to this operation. 

[akash.kamoolkar]

@Six1Seven1 Is this what you want to do?

Regards,

Akash Kamoolkar

[Six1Seven1]

@akash.kamoolkar 

Thanks for your file but I am unsure what that file is doing because the toolpath on that file on my machine still will not generate. 

Allow me to explain the real-world practicality of this matter and what is happening and why Fusion should be accommodating such need...

In this case, with the tool selected (right hand holder -35 deg diamond), a finishing op with this tool on the part profile will cause collisions on "walls" in the Z-axis.  This is less of a "Collision" but rather, extreme insert rubbing which will exhibit part issues and undesirable sounds from the cutter. I know this from experience, but even FUSION knows this. Because its highlighting the tool red when feeding from Z0 to back of part. See the attached image. 

[akash.kamoolkar]

@Six1Seven1 Have you updated to the latest release of Fusion that went out a couple of hours ago? This is the back to front toolpath I am getting.

Regards,

Akash Kamoolkar

[Six1Seven1]

@akash.kamoolkar Ahh that would make sense. Because my Fusion crashed in the middle of the update around 7:30pm ET.

Send your file again. Re-export it. I think you may have sent my original by mistake? 

[akash.kamoolkar]

@Six1Seven1 Here's the changed file again. I am also attaching one with the toolpath going front to back where the tool won't drag against the vertical wall (I checked the no dragging parameter).

Regards,

Akash Kamoolkar

[Six1Seven1]

OK were making progress.

So your files are from a newer version of F360 than me, so my update didn't go through.

First, the 'No Dragging' feature. I saw that and should have tried that. Thats interesting. I like that feature a lot actually.

Second, your changed file works kind-of. I like to run these finishing passes to X0 at the face of the part some times. Instead of adding a finish facing pass. Do it all in one finish turning cycle. Is this possible?

As for duplicating your results, I think *part* of the solution of your file is that you allow radial grooving, but you increase the Inner Diameter up to ~1.500" (avoiding the groove).

I tried this and I can't get the same result. See attached.

Thanks for your help

[akash.kamoolkar]

@Six1Seven1 in case of the back to front toolpath, for the tool to also machine the face of the part, the inner radius would need to be set to the stock / model ID. but this would unfortunately also make the tool to enter the thread relief groove, not to mention the individual threads as well. This issue should be resolved by the new groove suppression feature I mentioned before that we're currently working on. (FYI, the only difference between the file you sent me and the one I sent you is, I set the inner radius to "selection" and set the selection as the top of the thread).

So, a viable alternative for your use case would be to do a front to back no-dragging toolpath, grooving set to "dont allow grooving" front limit set to "stock front" and inner radius set to model / stock ID. I have attached the file.

Regards,

[prkdesign14]

Hi Akash,

I am having a similar problem, maybe you can help me...

I would just like to machine a chamfer and face the part in one operation.

so lead in at 45deg from the back, complete the chamfer and the proceed to face the part and lead out at 45 deg again.

it seems to ignore the facing part and just moves to safe position once the chamfer is done.

[akash.kamoolkar]

@prkdesign14 can you attach your file here?

Thanks,