Tool movements are backwards

[billbarschdorf]

Hi all,

Trying to resolve an issue with tool orientation after posting. I posted another question about this here, got to a point but that thread now has gone dead but I still do not have it resolved.

Here is that post.

https://forums.autodesk.com/t5/fusion-360-manufacture/tool-path-will-not-generate-with-tool-orientat...

My machine is a Sherline chucker lathe which is a gang tool lathe. My control is a Centroid Acorn running CNC12 software and Centroid turning post.

https://a360.co/3Gi6Its

The issue is when running the job on the machine the tool movements are backward for my cut-off tool. It rapids directly into the endpoint of the cut then pulls back. I need it to rapid just above the part/stock, plunge straight down in +X, make the cut and retract straight out in -X. It's not doing what you would expect. Its starting the cut in +X.

I have my tool set to bottom side orientation and defined as a turret tool with 104 in tool set up as per Fusion tech support.

The issue is the centroid post is not doing whatever conversion it needs to for the orientation. SO how to get this all working?

The guys on the Centroid forum are saying program with negative numbers but im not exactly sure what values to change in Fusion? IS this the only thing I need to work out OR do I need a custom post processor?

I have a video on the Centroid Acorn forum here, (bottom of the page) please note the job it's running has a groving operation and cut off in the video. Notice how it starts at the bottom of the cut.
https://centroidcncforum.com/viewtopic.php?f=60&t=6345&start=50

[Richard.stubley]

Hi @billbarschdorf,

My feeling is the rotation vector is wrong. So where you have A=1,0,0 it should be A=-1,0,0.

Are you using the machine configuration or do you know if this is hardcoded in your post?

[billbarschdorf]

My feeling is the rotation vector is wrong. So where you have A=1,0,0 it should be A=-1,0,0.

What is the rotation vector? Is this referring to the tool? I really don't follow. 

Are you using the machine configuration or do you know if this is hardcoded in your post?

I have no idea

Maybe a bit more detail and explanation would help. 

[Richard.stubley]

Hi @billbarschdorf,

Looking at your project again, is it just the cut off that you are experiencing the issues with?

Does the cut off tool come in from a different orientation to the other tools?

[billbarschdorf]

Yes, cut-off comes in from the topside and that is a whole other issue in itself since Fusion does not support top side tool orientation currently. Supposedly the post is supposed to convert the orientation? BUT still trying to work all that out. 

Cut off tool is tool #9 

[engineguy]

@billbarschdorf 

Not sure if this is anything close to what you are looking for, seems to Simulate OK but does it generate the code you need OK ?? If not then you may need a Post Processor modification.

File attached and Screencast here https://autode.sk/3JbY0Pp

[billbarschdorf]

I dont get it?  The set up you did has as many or more errors than I have.  the tool is red which is the kiss of death for tool path generation,  in simulation the entry move is cutting through the stock, and then the cutting moves are also backward.  So not sure what your doing? Im I missing something or is my computer broken? LOL

[engineguy]

@billbarschdorf 

Don`t know what has happened to the file, it works fine here as you can see on the Screencast, maybe it is corrupted during the upload ??

Anyway, here it is again using a different Name, it still works as per the Screencast here !!

[billbarschdorf]

Ill take a look at home, thanks 

[billbarschdorf]

I took a look at your file and realize I should have not said TOP as in Z top/up and down top LOL but as in "top of the gangplank table.  I meant TOP of the table in X not literally TOP as in Z.  Im sorry I should have been more clear. 

[engineguy]

@billbarschdorf 

🙂🙂🙂  OK, got it now I think, have a look at the inage below,I just flipped it from 90 deg to 0 deg and also moved the Groove operation into the same setup as it is using the same tool. and changed the Setup to get the tool to the back.

If your code is not correct in the X- and X+ then just change the Turret designation under the "Post Processor" tab for your tool, looking at your photo I would think that the Face/Rough/Finish are moving in an X- direction and the Groove/Part Off are going in an X+ direction.

To get X- values for an operation then set the Turret to 103 for that tool and for an X+ value then set the Turret to 104 for that tool.

Hope these ramblings help 🙂

[billbarschdorf]

Interesting, so as I see it you've cheated the fact that fusion does not support simulations and tool path gen for top side tools by creating a 2nd setup and simply rotating the setup, that's cool. RIGHT? Its basically like we just rotated the machine 180? NICE is that what you were thinking?  Kind of a quirky workaround, I HOPE I remember this,  but it works and the simulation runs on my box.  Brillant approach!  Thank you I cant wait to run this on the machine and see if I'm out of the woods. This is a big step forward for me, much appreciated! I was thinking I may have to rework my entire table set up and relocate a bunch of tools to get the cut-off coming in from the X- direction (bottom side). 

103 for X+ moves

and 

104 for X- moves..  :  ) I had mine set to 104 as per one of the AD techs not sure why he did not tell me about 103? 

Will report back after I run the program on the machine. 

[engineguy]

@billbarschdorf 

No cheating, to use what is in effect two different "Turrets/Toolposts" then it would require a second setup, this is what is always done in my experience, if you had two actual rotating turrets one at the front and one at the back of your spindle that is as far as I know the correct way to approach your machine layout 🙂

Terminology can be confusing, to me your CNC has a Front and a Back, much like the Citizen Lathe with the Mitsubishi Control, that is how I have seen such a  Lathe setup by it`s owner a few years ago, I tend to go with what I know.

If you have your 104 (This should produce X+ values in the code) and 103 (This should produce X- values in the code) settings for the correct tools then you should be good to go.

I am sure that there are some expert Lathe users out there that can maybe give you a better answer, what you have is what I have, it is simple workflow to follow and just seemed like the easiest method to me  🙂 🙂 🙂

[billbarschdorf]

😁Will keep you posted thanks much

[engineguy]

@billbarschdorf 

Cheers, it will be interesting to see how that actually works out at the machine, nice to see someone prepared to come back and let the Community how it went, good or bad 🙂 🙂 🙂

[billbarschdorf]

Happy to report the program is running as expected on the lathe and all functions working.  YOU ROCK! I appreciate the help SO much Ive been trying to get this worked out for weeks, (after hrs from day job) all while learning everything else AND finishing up this DIY build.  A LOT of stuff to do and learn (new to CNC lathe) but not mill CNC and I really appreciate the dedicated help you provided on this.  THANK YOU!  I want to Cry I'm SO happy!!! LOL  😂😂😁 

I WISH there was a way to "store as template" for an entire setup, that would be nice. But will store the individual MOPs for reference and archive this post in Onenote for all my future (top/back side) tool set ups.  

thanks 

[engineguy]

@billbarschdorf 

Glad it has worked out for you, quite a project building that type of Lathe. well done 🙂

It is just one of those things that you can look at over and over and can`t "see the wood for the trees" situation, been there often, really stuck on something and then someone just walks past and says something like "why don`t you just do so and so", then it all comes clear 🙂 🙂 🙂

As long as you have those two small programs I posted to refer back to, the more times that you program things will get easier, of that I am sure 🙂

Good luck with your Projects 🙂 🙂 🙂