Need help with setup for turning (Z axis backwards?)

[Anonymous]

So I'm trying to set my CNC mill up for CNC turning (with the part chucked into the spindle).  I've created the below test part.  You can see the extra stock on the left end where it would be chucked into the spindle (round end facing down towards the table).  Origin is set to "stock front".

Screen Shot 2019-04-25 at 7.33.29 PM.png

Ok, so you can see the Z axis is pointing down towards the table.  Normally when I do CAM for milling operations the Z is pointing up towards the head.  As it is the tool is oriented correctly with respect to the spindle rotation.

Screen Shot 2019-04-25 at 7.34.03 PM.png

But if I flip the Z axis in the setup it also flips what is front/back of the stock/model.  This also results in the cutter being backwards with regards to the spindle rotation.  See below.

Screen Shot 2019-04-25 at 7.41.24 PM.png

I'm confused how to set this up correctly.  I can probably account for this in my machine settings but it would be nice to not have to switch machine configurations between operations.

Somebody tell me the setting I'm overlooking :).  Thanks!

[Boopathi_Sivakumar]

@Anonymous 

f2.jpg

Z axis will always points outside towards the center. Based on the turret tool position the X axis may vary but the Z+ will always points out in CNC's . In your case the first setup is the right one.

Thanks,

Boopathi

[Anonymous]

I would agree that first setup is correct, in addition, Z axis in setup needs to point in direction tool is coming from.

For this to work on mill, you may get the toolpath but post processor will most likely produce "Tool orientation not supported" error.

I would suggest programming this as a lathe job, resulting code will feed Z axis in minus direction, you would then mirror Z axis including K values in arcs and reversing G2 / G3 addresses in NC editor.

As a result, your mill would make a cut in Z axis positive direction while spindle physically travels in Z minus direction and towards the table, have Y axis at zero at all times and work X axis as a turret on lathe.

Initial code for tool change, speed, feed and such will have to be adopted to mill, but I think it's doable.

I would also suggest using 35 degree insert to gain more access in arcs and on center line of part face.

https://www.cnc-syntax-editor.com/

[seth.madore]

I'd also give this thread a read. It's interesting to see the whole "where there's a will" mentality in makers 🙂

[Anonymous]

Thanks (everyone) for the replies.

When you say to program this "as a lathe job", what do you mean? Use a lathe post processor?

I'm surprised there isn't an option for this in Fusion since it seems to be somewhat aware of mill turning (it's mentioned in the setup options).

I may look at copying the post processor I'm using (EMC -- for LinuxCNC) and modifying it to flip the Z coordinates.  I'm very inexperienced with G code, but at least I have software skills.

[Anonymous]

This got my crystal ball overheating, so let me try this while standing on my head, you can't feed table up, so you must feed spindle down instead, which means programming it as standard lathe job.

You will feed spindle on mill as you would feed turret on lathe but code should be the same as far as X and Z is concerned, negative Z coordinates starting from rounded face of part as Z0.

That leaves you with editing top and bottom of code to adopt it to mill, and changing feed mode.

[johnswetz1982]

@Anonymous  "I'm surprised there isn't an option for this in Fusion since it seems to be somewhat aware of mill turning (it's mentioned in the setup options)."

It is not Mill Turning like you are describing in this post and some others have done as well. A Mill/Turn means a lathe with live milling tooling like a DMG NLX or a lathe with a milling head and tool changer instead of a turret. Something like a Mazak Intergrex or a DMG NTX.

[Anonymous]

Thanks for the terminology clarification.

[Anonymous · Accepted solution]

Well ok so I went down the path of flipping the Z direction on my LinuxCNC configuration to work with what I was expecting the CAM output to be.  I did a couple tests and found that the part was coming out upside down.  Very confusing.  I went back to my normal machine configuration and everything worked fine.  

For reference, I am using this LinuxCNC turning post processor:

https://cam.autodesk.com/hsmposts?p=linuxcnc_turning&_ga=2.25101694.512629405.1556382885-432165678.1...

As far as I can tell that works great.  The part didn't come out exactly perfect but I think that's a workholding issue.  Thanks for all the responses.

[daniel_lyall]

It is mill turn there are a few ways to do it, the Linux or path pilot post just needs a change done to it. Don't ask me how the person who showed it did not say how to adjust the post they just said google it.

If you lay the machine down so the Z axis is on the ground and the Y is pointing up it looks like a lathe. The tool holder can be the vice or something you make to hold onto the tool.

And yes the Z needs to go backward for it if the material is in the spindle if you are using The 4th axis as a spindle it is the X that becomes Z.

A few Linux and Mach3/4 users have changed over to path pilot.

Can you post the model you got working I would like to have a look at your settings? To do this Go to File -> Export and save as a .F3D Archive File and attach it to your next post.

[Anonymous]

Whether Z direction is positive or negative depends on where you set origin.

If origin is set at rounded end of part, Z will be negative, tool clamped in wise, Y axis at zero at all times, you feed spindle down towards table while moving X axis to machine contours at the same time,........... Z (spindle) moves in minus direction, just like on lathe with Z zero being front of the part.

Driving spindle up and down becomes same as driving turret in back and forth in Z axis of a lathe.

Program as lathe job, adjust initial code to run on mill (tool change, feed per minute etc)

If you set origin at back of the part next to spindle, Z will be positive because spindle travels up and away from table as tool progresses towards rounded end of part.

Program as above and mirror Z axis.

[daniel_lyall]

I always get the Z around the wrong way on lathes, I dont use them enough.

[Anonymous]

My file is attached.

[Anonymous]

I changed few things, you want to finish front radius while rest of the stock is intact, cut from outside toward center in  light passes, rough OD and do 3 finish passes to get clean finish, then finish groove using 1/16 wide insert.

Feeding tool into center line is bad idea, no surface speed there, it would chatter badly and ruin insert tip.

Using 35 degree insert, .015 radius for less tool pressure, tool is tilted to have negative 1 degree face clearance, this allows full access of back edge in undercuts.

I posted for lathe then changed all X diameter values to radial, you need to adopt it to your mill.

Z0 is tip of front radius, set tool on positive side of X axis and about .005 above center line of part, this will compensate for stock deflection and minimize chattering.

Part should be oriented in spindle so that radius points at table. 

Have fun and let us know how it works out.

2019-04-27 22_07_11-[] (C__Fusion_NC_1001.nc).jpg

[Anonymous]

Duh, forgot to attach  file.

[daniel_lyall]

@Anonymous  If you are planning to do this more often it would be a good idea to convert a mill/turn to work with Linux so you have a mill doing turning post.

I did A mach3 one a few years ago It was not all that hard to convert and having a Y0 saves having remember to do it before you hit cycle start one of the Fanuc based ones would be close.

[Anonymous]

There was no way to make same tool accommodate facing and back angle of front undercut, I overlooked that earlier.

I reset tool to normal, 3 degree face clearance and used .047 wide grooving insert to finish groove and back angle of front undercut.

I modified NC file to what I think is good to go, T1 is your stock, throughout program, after posting for lathe diameter, I made X values radial.

Attached are new Fusion and NC file.

2019-04-28 07_52_40-Autodesk Fusion 360.jpg

[daniel_lyall]

@Anonymous It pays to find out what tools the OP has otherwise you end up wasting your own time on something. This is just a comment do not read into it.

[Anonymous]

---

@daniel_lyall wrote:

@Anonymous It pays to find out what tools the OP has otherwise you end up wasting your own time on something. This is just a comment do not read into it.

---

Well I am going to read into it because my persistence may be misunderstood here, I make more money as a result of using Fusion and being on top of my daily activities.
Since when is reasoning part of the deal in machining industry? LOL  ............., well you see, some things demand right tool for the job or closest thing to it, and if you don't have it, you can get creative but it only goes so far, because sometimes what you have is not going to do impossible.

Now about "wasting time", ................ since I started pounding on things here, I learned a lot more then if I just watched YouTube videos. I don't just do things to "solve the problem", I learn better by poking with things and registering sequence of getting it done.

I discovered or confirmed bugs where I wasn't sure if one existed so nothing is waste of time to me.

In few instances I felt like throwing file away would really be wasted effort so I gave it to original poster instead, after all it already served purpose in my objective.

If it's not usable, discard it, nothing to explain or be intrigued about.