What's new
What's new

Is it possible to create an interpolation turning operation on ESPRIT 2020??

Leo Vergara

Plastic
Joined
Aug 10, 2022
Hello, community!
Does anybody know if is it possible to create an interpolation turning operation on ESPRIT 2020, and how??

With Interpolation turning I mean something like this:

Really appreciate your help on this!

Leo.
 
Hello, community!
Does anybody know if is it possible to create an interpolation turning operation on ESPRIT 2020, and how??

With Interpolation turning I mean something like this:

Really appreciate your help on this!

Leo.
When it comes to features like these that companies like DMG, Okuma, and Mazak like to flash being possible with their conversational control, I want to know what company that would have these million dollar machines wouldn't be using a programming department. Because in every case I've seen so far ,especially with Mazak, most of the features they like to say you are getting disappear when you aren't using the conversational control.
 
When it comes to features like these that companies like DMG, Okuma, and Mazak like to flash being possible with their conversational control, I want to know what company that would have these million dollar machines wouldn't be using a programming department. Because in every case I've seen so far ,especially with Mazak, most of the features they like to say you are getting disappear when you aren't using the conversational control.

It's easy with Heidenhain. What I did was I programmed the feature as if it were a regular turned part, extracted the toolpath X/Z coordinates and inserted them into the interpolation turning cycle that I programmed by hand. Then called that as a subprogram from my main CAM program. Simple. We are a small company too, only 8 machinists and we all program our own machines.
 
When it comes to features like these that companies like DMG, Okuma, and Mazak like to flash being possible with their conversational control, I want to know what company that would have these million dollar machines wouldn't be using a programming department. Because in every case I've seen so far ,especially with Mazak, most of the features they like to say you are getting disappear when you aren't using the conversational control.

A lot of the OEMs that buy these machines (and features) by the dozen are setting them up to make one part or one family of parts. Even the best CAM leaves a lot of cycle time on the table when your producing 100's of thousands of parts, so the code is typically some ugly amalgamation of CAM and notepad. In many cases the entire integration is handled either by the machine tool builder or a third party.
 
Hello, community!
Does anybody know if is it possible to create an interpolation turning operation on ESPRIT 2020, and how??

With Interpolation turning I mean something like this:

Really appreciate your help on this!

Leo.

I've just asked our senior milling engineer about this. Interesting, but technically incorrectly named. This is not turning, workpiece is not rotating.
I'll update when I'll get an answer.

I've seen boring done in similar fashion by our milling department, but it was MillTurn machine.

Usually problem with these "weird techniques" is that different people gives different names to it. And then we have a tragedy of Tower of Babel.

Like Thread Pecking(ESPRITCAM) <-> OptiThreading(Sandvik). Thread Pecking is technical name, while OptiThreading is fancy trademarked name, but its doing the same thing.
 
Last edited:
No CAM system can do these type of programs yet. DN Solutions has conversational programming on the control to use Fanucs CS TurnCut. I have done demo in an NHP5000 successfully. Pretty cool but definitely a niche tool. Useful for large parts that can't be done any other way.
 
No CAM system can do these type of programs yet. DN Solutions has conversational programming on the control to use Fanucs CS TurnCut. I have done demo in an NHP5000 successfully. Pretty cool but definitely a niche tool. Useful for large parts that can't be done any other way.
Doesn't that need some factory upgrades? Way back when, I had to get a HMC that had a bunch of factory hardware options to really make it live. The Y axis ballscrews can burn up.
 
No CAM system can do these type of programs yet. DN Solutions has conversational programming on the control to use Fanucs CS TurnCut. I have done demo in an NHP5000 successfully. Pretty cool but definitely a niche tool. Useful for large parts that can't be done any other way.
I can't speak from first-hand experience with this, but according to the What's New, this is possible in TopSolid 7.16....would be curious to hear from folks who have tried this out.
 

Attachments

  • Whats New-Interpolation Truning in TS 7.16.jpg
    Whats New-Interpolation Truning in TS 7.16.jpg
    136.2 KB · Views: 18
I can't speak from first-hand experience with this, but according to the What's New, this is possible in TopSolid 7.16....would be curious to hear from folks who have tried this out.
Nice, glad to see someone is listening. The Fanuc option is a nice niche tool that would come in handy on a lot of parts. I know Seimens and HH have this also. Getting this into mainstream CAM is a good thing.
 
Last I looked into this, the AE said it was not overly accurate. Nothing CAM related but more of a machine limitation with all that's going on in a cut like that. Anyone have knowledge on surface finish/size +-/consistency? It was the last IMTS I looked at a machine doing this.
 
Hi gooose:
You wrote:
"it was not overly accurate"

Yeah when I look at the example I go "why bother".
It's a workable solution to a very small subset of problems, I suppose, but for the example chosen for the demo, it's one of the stupider ways I've encountered to make those features.
If they's shown a big casting with a goofy shaped boss on one corner...something you'd never swing successfully on a lathe or a VTL and with a shape you cannot mill or reverse bore, I'd probably perk up my ears, even though I've never had to do it in forty years.
But for this? Naahhh!

So if it's not even accurate, (aside from being stupid for that particular job), I can't see rushing out to buy it.
As far as writing code to do that with Esprit I have no idea but I doubt it.
It looks like a conversational cycle resident on the machine control.
You could probably roll your own if you had a machine with spindle orient and too much time on your hands.

I've seen videos of standard machining centers with CNC boring /facing heads that can do the same sort of work.
I have also no idea if they can work more accurately than this method, but they've been around for a long time.
I also don't know how they're programmed.
I believe they can get a lot closer to the proper surface speed for the carbide inserts too.
Here's a link:

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
I've done quite a bit of this on Mazaks, we call it Orbit Turning. It's G code only, but there are a couple nice features on the control that make it easy. What I've done in the past is program the feature as if I was doing it on a 2X lathe, then add the needed start and end codes to make it run on the mill. I haven't seen any CAM software offer it out of the box yet, hopefully that changes in the near future.

As far as accuracy, it is a lot better than you might expect. You're not gonna hold 0.0001" on a diameter, but I've had circularity come out in the 0.0005"-0.001" range on an un-tuned machine in the field. If you order the option from the factory it gets some extra time with a ball-bar to adjust the servos.

The main 2 reasons these kind of operations are practical are reducing setups and surface finish. If you have a feature that requires a turned finish it is a no brainer. I have a customer that loves it for finishing ports vs having to get a bunch of custom form tools. Setup reduction can be huge, I helped another customer with a big titanium part that required 8+ hours on a VTL with an eccentric fixture to make 5 offset bosses. We were able to use orbit turning on a vertical Integrex millturn to eliminate that whole operation. Even with the much slower effective RPM we were running in orbit turning, the operation could be completed in under an hour on the Integrex, as well as combining it with other traditional milling and turning operations on that machine.

If you need the fastest cycle time those D'andrea U-axis heads are the way to go. But having priced them out myself for several projects, you're looking at $30,000-100,000 once all is said and done for the style that can go in a regular machining center. The orbit turning option is about $3,000.

Here's an example of what the code looks like for a simple boring operation.

<ORBIT-BORE>(ORBIT TURN ID BORE)
G00 G90 G59
G18 G40 G80 G95 (G18 NEEDED FOR ORBIT XZ PLANE)
M194 (C/V SERVO OFF)
G90 G53 Z0.
G0 A0. C0.
(G91 G28 X0. Y0.)
T10 M6
G90
G43 H10 X0. Y0. Z4. P1 (INITIAL POINT)
G61.1
M193 (CONNECT C/V-AXIS)
G0 V90. (ORIENT TOOL TO 3 O'CLOCK ON BORE)
G90 G0 X2. Y0. Z.5 (MOVE TO START POINT)
(G97 S100) (IF NO CSS, SET RPM)

G10.9X1 (DIAMETER MODE)
G148 X0. Y0. (ORBIT MODE ON, SET TURNING CENTER POINT)
G96 S100 R3 (CSS ON)
M764 (ORBIT FORWARD OR REVERSE)

(BORE ID)
G94 G00 M08
X4.
Z.25
X4.251 Z.071
G95 G03 X4.375 Z.009 I0.0 K-.062 F.0047
G01 Z-.491 F.005
G03 X4.317 Z-.52 I-.029 K0.0
G01 X4.2747 Z-.4973 F.0053
G00 X4.2626 Z-.46
Z-.45
X1.358
Z-.458
G02 X1.482 Z-.52 I.062 K0.0 F.0047
G01 X4.317 F.005
X4.2747 Z-.4973 F.0053
G00 Z.25
X4.

M9

G40
M765 (STOP ROTATING MOTION)
G149 (ORBIT MODE OFF)
M194 (DISCONNECT C-AXIS)
G10.9 X0 (X RADIAL MODE)
G0 Z2. (RETRACT)
G0 G53 Z0.
G0 G53 X0. Y0.
M30
%
 








 
Back
Top