What's new
What's new

Onecnc Lathe, any users here?

SND

Diamond
Joined
Jan 12, 2003
Location
Canada
I'll likely get the Lathe Express module so I can get up and running parts quickly but I was just wondering, when it comes to things like bar pulling, parts catcher function, or custom tool holders for weird ops. Can you do all that with the cad/cam program, or do you have to hand code those lines into it? I'm slowly starting to work on properly learning G-code and I sometimes tweak my mill programs a bit by hand, still not very confident but I'm working on it, slowly....

So, any Lathe user feedback would be great, unfortunately there's not nearly as many lathe tutorials as there are mill tutorials, those were a huge help to me.


thanks
 
What version?
I have XR5 lathe, and I'm not a fan.
The software (at the time...) seemed to be an afterthought. "Oh, we need a lathe program too! Ok, I'll just change the name of the X axis to be a Z axis. Yeah! That's the ticket!"

My version is/ was pretty unrefined. Read: Not near as much thought put into the lathe side, as the milling side of the program.
I would not purchase it again....
Having said that...

The post is still really easy to configure, so I would imagine setting up Bar Feed, Parts Catcher, etc should be easy to set up:
Either by "insert code here" in the program, or specifying a M or G code in the post processor.
If you know the milling side, then the lathe side is kind of a breeze.
 
Newest would be XR7.
Seems most cad/cam programs mostly focused on mills, lathes not to much.
I like that the post in Onecnc is user adjustable unlike most others, an no maintenance fee.
The mill version has been a huge help to me, I'd have been screwed without it.
Now, the lathe does come with Fanuc GuideI, so maybe I should test what it does too, but I'd rather sit to program than stand at a machine.
 
I got there mill express a couple years ago ( XR6) and could not be happier with it ,,, Its simple and works vary good for fixture work ,,, the
part programs I still hand code so I can get them to run faster..

I would contact Onecnc and do there 30 day free demo of it ...
 
I have had lathe express XR5 through XR7. The mill software is more sorted than the lathe software. As far as the parts catcher, tailstock, and bar pulls, add the custom code icon to your toolbar, and write those options in there so you don't have to edit it into each program. Custom tools are pretty easy to add to the library in XR7, big improvement since XR5. As D.D. said get a 30 day demo.
 
So, for you guys using it. Is there a trick to making it post a M04 CCW spindle rotation? I'm only getting M03 to post.
Also, any way to remove the decimal point from P and Q when it posts? I want it to be say P1000, Q0500 now its doing Q.05, control ain't happy with that. I could hand edit but there's gotta be a way, tried many things with the post but no luck yet.
Is this what the custom V1, V2, V3, V4 are right beside the tool selector on the first page when doing toolpaths? I'm not sure yet what those custom things are, custom tools maybe? its a lot to learn in not much time...
 
So, for you guys using it. Is there a trick to making it post a M04 CCW spindle rotation? I'm only getting M03 to post.

I had the same issue. The Fanuc post I had started with posted M03 for every tool. You need to edit the post. Remove the M03 from the "Turn Tool Format" and add the "Tool-Spindle CCW" and "Tool-Spindle CW" codes in its place. (They can be on the same line.)
 
Tried that yesterday and it didn't seem to work but I'll try again.

Any guess on the decimal issue? and what the V1 V2 ... custom things are?
 
Tried that yesterday and it didn't seem to work but I'll try again.

Any guess on the decimal issue? and what the V1 V2 ... custom things are?

V1, V2 are custom variables. You can see them in the long list of Insert and Substitutions in NCsetup, under the Posting Format tab. They are called Tool-CV1-Option1 and so on. The little box at the bottom called "Prefix" is where you can hard code the value that is associated with that variable. There are 16 options listed, and you can use them for any special M codes or G codes, or anything within reason, I suppose. You have to write in the Prefix what you want, and you have to insert that particular variable into the desired location in one of the fields on the left side, where you are editing your post format for a particular purpose.

As for no decimal, I'm not sure which thing you might be setting up, but if you place a space character after a number, then OneCNC won't put a decimal after the number.
 
Thanks, all.
I just talked with Mike at Onecnc, excellent customer service, it was quite simple to make the right adjustments and all is fine now. I also better understand what to do with the custom functions now so I'll probably make a bit of use of it once I get a bit better with the machine.
I had a similar issue with my mill giving an error on the dwell numbers before, so now I can fix that one too I think, even if its really rare I need to use dwell for my work on the mill.
Although my new machine game with a pretty good control and great simulation/code checking capability before running anything, I really like the onecnc simulations and ease to tweak stuff for someone as inexperienced with cnc as I still am.
 
I just talked with Mike at Onecnc, excellent customer service

Mike is GREAT!
Honestly, my referrals for OneCnc (milling side, only) are because of: [in order of importance to me]
excellent customer support
the ability to sell a copy
no maintenance
ease of changing the post
finally, the program itself. :DLOL
 








 
Back
Top