CAM for lathe? What are folks using successfully?

Ok, so I'm looking to get some older 2 axis iron and retrofit it with an EMC setup - nothing too fancy - probably in the size of a small Wasino or an older Okuma. Due to some recent shop construction, I don't have room for the larger Mazak I was going to get (might even have trouble fitting in a QT-10!) - but that's another matter entirely.

I have programmed CNC turn centers before by hand, and have used (at another facility) both Gibbs and BobCad for turn, but none of that is available to me now. And to be honest, I'm more of a VMC guy, anyway. (Rhino and VMill for a lot of years)

That's a long intro to the question: for those EMC2-Lathe users out there, how are you getting your 2D (DXF or equivalent) contours into EMC (or any other control for that matter), including either control-canned or cam-canned rough/finish passes, threading and parting cycles?

I've reviewed the (albeit short) wiki list - of course it is quite heavily mill-centric. A lot of the new controls (one of the big Okumas we considered, for example) will take in DXF profiles natively, plus with turn-mill and live tools, what used to be a simpler "contour following" process can now almost require a custom piece of software for each machine, thus I can understand why a lot of folks rely on the conversational options on their controls.

So - here's a great test for this new part of the forum...what's ye folks got under the hood?

Cheers,

Ted.

Hi there

we are going to start retrofitting out our laths very soon in next 2 weeks or so, we have two Hardinge superslant twin turret laths, 16C collets etc.
as you say EMC has no "routhing" cycles as of yet, to turn down a diamiter on bar or routh to 4/5points or more on a contour it is something i have been looking at and seeing if its something i could look into helping out and adding in.

anyway back to your question.
we here use CAM to program anything complex in shape we use Camworks, it can do full out as u say, sub spindle, live tooling, C axis and more but u sure pay for it.
we have always looked at many cam systems but when u say to them what about turning they always seem to run for the hills, or they say yes we have it and thats it.

rob

BigJohnT wrote:

Rob,

Do other lathe controls have G-Codes for roughing or is it some conversational part of the control?

John

hi john

it varys abit from control to control fanuc onces are pritty good, but so are the ones in the philips controls.

all you basicly do is use a G code to call up clearnce cycle, defind any end points, rads, finish pass ammount etc and it will work out all the intersect points and follow the contor for you.
these days cad/Cam makes it quick and easy and find your self spitting it out long hand on cam systems. but alot of time u some times just want to routh down a bar to asize or a quick simple profile. which is where cycles come in.

eg
G70 (Finishing Cycle)
G71 (OD or ID turning cycle)
G72 (Facing Cycle)

check this CNCzone post i found just now
www.cnczone.com/forums/showthread.php?t=12002

shows the basics
i do have a few in long hand varible gcode some where. so u can see how they work it all out etc.

rob

For turning, we've been using Dolphin Cam V10 with ok results. The software is not very polished, has some intermittent bugs when it creates the g-code but is otherwise functional. V11 just came out and not only is it substantially cheaper, the user interface looks much better and I would guess they have fixed some of the bugs. If we decide to upgrade to the new version I'll post regarding that.

We mostly use it for reprofilling railway wheels in the following fashion:

Use a large house-made pin gauge to get an impression of the wheel as-is.

Place the pin gauge on a scanner to get a jpeg that reflects the wheel shape.

Import the jpeg into AutoCad and scale the image to match the units correctly.

Create a spline that matches the end of the pins.

Line up the spline against another pre-made spline that marks the finished profile to come up with the material that needs to be cut.

The finished-profile-spline should be below (in terms of y) the as-is spline and they should both be referenced to a known point in Z (we use a point on the machined disc wall as a reference).

Export the two referenced splines as a dxf.

Import the dxf in Dolphin Cam.

Tell Dolphin Cam which spline if the finished profile and which is the as-is profile.

Select your tools and create your job.

In all its a pretty easy software to use and so far we are pretty pleased with it.

Hope that helps.

Frank

John -
Although I may have been feeling "6 feet under" on occasion, I'm hoping it wasn't that bad. To be honest, the forum still hasn't seemed to have taken up the reins from the mailing list like one may have wished. That, and there really wasn't any real activity to the post!

To answer my own question though, I've migrated to SprutCam (Master) for my needs with my Mazak mill, (4 axis, g code, no Mazatrol, thank you!) my Tsugami lathe (with C and live tools), and my Mitsubishi laser table. The Tsugami lathe is the only unit that has LinuxCNC on it; the other machines still have their original controls.

What I like about SprutCam:
- great postprocessor editing capabilities - for a "coding guy", I like the fact you can get deep under the hood. Not as simple or straightforward as VisualCam (my old cam system), and if you're not into coding, it can be daunting, although Tormach/Sprut will help you out greatly
- good tool library - lots of options
- rather good series of machining ops.
- allowance for trichoidal paths. Although some users don't use it, I use it a lot for rough milling since I have high speed capabilities on the Mazak. Keeps the cutter load really constant.
- simulation is excellent, almost rivals VeriCut. Not quite, but almost.
-Tormach is the USA reseller and have really run with the local support and training videos.
-support contracts aren't too expensive, and to date have been quite worth it!

What I don't like about SprutCam:
-part orientation link between Rhino3d plugin and lathe always turns out wrong. It's fine when I import an iges however. And I prefer to keep CAD and CAM files separate, anyway.
- simulator editing (to create your own machine) is a PITA if you don't buy the extra machine creator. I didn't see the point to buy the ability to create any and every machine when I only had a couple changes for my one. It's a module aimed at resellers and service bureaus, not the end user. If your machine is already simulated, it's not a problem, however. And there's a pretty good list.
- grouping machining ops for simulation or output (ie. skipping parts) is not as friendly as it was with VisualCam. But it's a minor irk.
-hardware dongle. I hate USB keys. As a developer, I understand the reasoning, but I still hate them. I'm a mobile, laptop-kind-of--guy and those things either get lost, or destroy USB ports when they get bumped. Still, not a gamechanger.
- Sprut update site is not always up. Sprut Forum is not always up. But they're doing better. Slack has been taken up by SprutAmerica.
-hardware licensing drivers and license file seems to become broken on every other update. It's fixed by an email to support. Probably just waiting for the "next generation rewrite" for it to disappear.
- can be difficult to split tool offsets between the control and the CAM; I like tool radius offsets to be done by CAM, but tool length offsets to be done by the control. More often you don't need to substitute a 1/8" cutter for a 1/4" one, but do need to replace a 1/4" with a 1/4". With a toolsetter on my Mazak, I prefer it to change the length offset there, instead of having to go back to the CAM and repost. I don't like running no-radius offset from the CAM, as it doesn't simulate properly, and the Mazatrol tool table can get confused with custom tools and its own radius offsets. If the post processor in Sprutcam isn't written correctly, the offsets don't get called correctly. BTW - if you have a Haas, this is the CAM software for you.

Ted.

Cambam has lathe fuctions now. Free for first 40 uses and then 500 line limit if you don't buy it.
www.cambam.co.uk/forum/