learning 5axis mill with turning

[lowcountrycamo]

What do I call this?  Not really mill turn right?  I have a Postablitly  post.  Should I set this up as a VTL?  My vericut sim should support this but the sim looks wrong.  I am very frustrated as I cannot really find any good info as to how to make this work.  I reached out to our reseller and got a link to a Postability video that did show a little, but not nearly enough.   

Any help would be a blessing.

 

thanks

steve austin

[JParis]

It is a Mill-Turn...

The configuration either has to be as a Horizontal Lathe or a Vertical lathe...it's impossible from here to tell you which the post is set up to handle by default.

 

It should have come with a Machine & Control defs as well...look at the machine def and see what the planes setup is at this point

You might want to open the post and read some of the notes inside..

You "may" be able to set it up as either but learning what the post is doing is the important part of that...

A picture of the machine itself might help someone set you down the correct path

[lowcountrycamo]

sorry for the missing info.  It is an okuma MU6300 VL.  A C trunnion.  I should be cutting in the y axis at A0. or A90. I believe.    I general program from COR.  To continue that should I touch off lathe tools using the probe or take a cut and zero?

 

Thanks

[Greg Williams]

Uplaod a file, happy to look

[cncappsjames]

I have programmed a Matsuura CUBLEX-63. This is also an A/C machine that cuts in the Y direction at A0 and A+/-90.

I set the machine up like a VTL because when everything is at home, that's what it is. I use CAMplete for my Post Processing/simulation solution and it uses/keys off info in the Tool Setup for determining A0 turning or A+/-90. turning. 

[crazy^millman]

Like JP and James had said setup like a VTL and use the LMD and CMD before doing anything. Move your model to top/top/top like you are going to program it. Then  program you milling operations using the top/top/top. I am programming for other companies so I program. I layout my planes in such a way to communicate to reflect how to setup the part. I copy top/top/top and rename it to the workoffset I will be using for that machine. Then I create my relative planes from it using the new linking process connecting them together. Use your stock models as you need and remember the lathe process to create solids to use through the operations. 

[lowcountrycamo]

All go info.  Thanks guys.  A year or so ago when we got this mill I was interested but never programed a turned part.  At that time Greg Williams was kind enough so give me a program he did.  That has helped a great deal.  One thing I cannot discover is how he altered the A axis cut.  as in these to pics.  It appears to be the same tool.  Could it be controlled with a misc?

 

Thanks

[crazy^millman]

The tools have a Tool angle in the tool command. It will be here that controls this. You can flash a tools also where you are cutting OD with it at 0 then can flash 180 and cut the ID with the same tool.

[lowcountrycamo]

Thanks  for that.  However, when I post this I get the tool cutting at a-90. z- which shows it cutting on the wrong side of the diameter in Vcut.  Does the machine expect code like this:

IF [VTLCN EQ  ] 
T3 M06 (ROUGH RIGHT - 80 DEG.)
NT3
G30 P1
M19 RS=0
G00 G19 G90 A-90.
M540
G197 SB=280 M503
G431 Z1
G433 H3 Y2
X0. Y-9.6955 
Z-.9995    <-----------------------------------
G196 SB=200 X1 M503
G95 G01 Y-9.5955 F.01
Y-9.3155
Y-9.3862 Z-1.141
G00 Y-9.6255
Z25.

[cncappsjames]

Just now, lowcountrycamo said:

Thanks  for that.  However, when I post this I get the tool cutting at a-90. z- which shows it cutting on the wrong side of the diameter in Vcut.  Does the machine expect code like this:

IF [VTLCN EQ  ] 
T3 M06 (ROUGH RIGHT - 80 DEG.)
NT3
G30 P1
M19 RS=0
G00 G19 G90 A-90.
M540
G197 SB=280 M503
G431 Z1
G433 H3 Y2
X0. Y-9.6955 
Z-.9995    <-----------------------------------
G196 SB=200 X1 M503
G95 G01 Y-9.5955 F.01
Y-9.3155
Y-9.3862 Z-1.141
G00 Y-9.6255
Z25.

But have you determined with the highest degree of certainty that Vericut is correct?

[lowcountrycamo]

No.  I would have to run the mill to be certain.  However I have programmed many mill parts on this machine and  I know z- is below centerline.  I looked in the machine manual, it specs mcodes pertaining to this function.  It did not give code examples.  Thanks

[lowcountrycamo]

G431 enables "turning mode"  If I where cutting this feature with an endmill z+ would take me there.   Reseller is checking on it.  Thanks

[crazy^millman]

What axis combination are you programming the turning with? Did they supply you with a Left or Right Turret LMD? Are your turning chains on the correct side?

[Greg Williams]

9 hours ago, lowcountrycamo said:

It appears to be the same tool.  Could it be controlled with a misc?

That file dates back to 2009, at the time there were not many options for posts. I hacked up a 2 axis Okuma lathe post, set it up as a 2 turret VTL, even though the machine obviously only has one turret.

 

I also used Misc values to output the Tilted turning code and the quadrant code, the plan was to use it for demo's.

[lowcountrycamo]

Greg that is clever.  I also attempted something similar when I was going through Colin's Post editing class.  I had some success but not enough to run on my bosses new machine.   And at the time I did not have Vericut to prove out. 

I have made some progress.  My reseller is contacting Postability.    It appears to me that if I select a horizontal tool I get A0.   If I switch to a vertical tool, A-90 is output.  However, when using the mastercam to vericut interface the A-90. tool comes it 90. degree off and backwards.  Here is a screen shot from mcam and vcut.  

 

 

[lowcountrycamo]

I contacted Vericut about this behavior and this is there response:

Steve,

I think the Mastercam interface is doing it’s job in translating the tools from Mastercam to VERICUT exactly as they are defined in Mastercam:

We are by no means Mastercam experts, but I would think that using a different Tool Plane for the operations that are tilted would be a more elegant way to handle that in the software. I’ve included one of my coworkers (Steve ) that has more Mastercam experience. He reviewed your files with me earlier.

I think that if this behavior will continue to be “hard-coded” in the post based on the tools’ vertical/horizontal orientation, you are better off building a tool library directly in VERICUT. To that effect, review Training Session 11 to see how to handle importing STP models of turning tools.

Please let me know if there is anything else that I can be of assistance with.

[crazy^millman]

I have been using 3D tools with no issue in Mastercam the old stick tools act differently than them and I wouldn't use them with Vericut. The interface will get a little wonky with the X-Y-Z values for Vericut. I will copy the imported insert and then make a Vericut insert. Pay close attention to the side the insert is facing. You can put negative values in the insert definition to flip it.

[Greg Williams]

My thinking is the machine can turn in both X+ and X- so why not set it up as a 2 turrett, We could then go the next step and say all right turrett turning is at A-90

[crazy^millman]

11 hours ago, Greg Williams said:

My thinking is the machine can turn in both X+ and X- so why not set it up as a 2 turrett, We could then go the next step and say all right turrett turning is at A-90

Greg on smaller parts yes, but on larger part that would be hard. The problem is the 3D tool is not respecting the machine definition for defining tools. We have Top and Bottom listed for turrets and not Left or Right when building 3D tools for VTL machines. The old school tool manager does reflect them when building tools. Then Wireframe tools from Mastercam act completely different than 3D tools so trying to use both in a programming project is a nightmare.

[Greg Williams]

I can get it to work in my 2 axis environment, but getting it to work and respecting the A axis in the post writers environment may be different. I dont have a Postability or In-house machine and control def to test it on.

I am not saying what I have attached is better or worse it is just what I have.

 

AUSTECH2009-MU500_TURNING-ISSUED.mcam

The vid from 11 years ago is here

 

https://youtu.be/6VYYIc8EFec

 

and here

 

https://youtu.be/M2Cs0PWyKXU

 

[crazy^millman]

Greg I remember these videos when you first did them. Yes the software has come a long way to handle these machines.

[Metals and materials]

Any videos or tutorials anyone know for mill -turn? 

[crazy^millman]

3 hours ago, Metals and materials said:

Any videos or tutorials anyone know for mill -turn? 

Caminstructor has a whole series on it.