New to mill-turn

[Bob W.]

Okay, I have taken the plunge and bought a new DMG-Mori NTX2000 with all the bells and whistles.  It has the B-axis head for 5-axis milling and turning and also a lower turret with live tooling and a Y-axis.  Also has twin lathe spindles (right and left chucks), part unloader, bar feeder, mist collector, and high pressure coolant.  I bought Mastercam's mill-turn to program this and so far it isn't going well.  Based on what Mori's AE said we also went ahead and bought Esprit.  He said typically it takes MONTHS for Mastercam users to get the post fixed to the point where they are getting good code without a xxxxload of hand edits.  What have others out there experienced?  I will be learning both software packages so it will be interesting to see the differences between the two.  Maybe I'll make a series of Youtube videos...

Right now mastercam isn't posting the tool number correctly and I can't even open the control definition to poke around, LOL!  In my opinion one of the biggest strengths of Mastercam is the ease of which users can modify and customize Mastercam and the posts to suit their needs.  It is a real bummer they have the mill-turn stuff so locked down.

[#Rekd™]

10 minutes ago, Bob W. said:

typically it takes MONTHS for Mastercam users to get the post fixed to the point where they are getting good code without a xxxxload of hand edits.

That is horrible.

 

[JParis]

I've had post fixes and adjustments in MT in under a day

 

[crazy^millman]

Bob good to see you. MCAMNW  one of the best resellers to handle this if anyone can. Reach out to them and you have my number if you need help getting up to speed. The MT machines have gone through some major overhauls as of late and programmed a Triple Handle Part for an Integrex I-400 using a Lower turret with part rest, steady rest and live center and it went really well. 

In the consumer part of Code expert there are ways to control your tool output. Have you looked in there yet? Also in the SYNC Manager pay attention to the settings.

[Bob W.]

Okay, that is encouraging.  I have no experience there, just going off what I have been told by the machine AEs.  Currently my post is outputting the wrong tool number (T7005 when it should be T6005) and the G41 command is on the same line as an XYZ move which doesn't seem right.  Any thoughts?

G41 X3.332 Y3.445 Z1.5

 

 

 

[Bob W.]

I have a call in but haven't heard back yet.  Right now I'm just trying to get usable code with the upper turret.  I have done extensive programming of 4 and 5-axis machines so the indexing aspect should be pretty straightforward.  What WCS should I use for setting up my parts?  For my HMCs I have always set the parts up as the machine is and created planes for B-axis indexes as opposed to setting it up to use Mastercam's right and left planes for 90 degree indexes.  I would like to do the same for mill-turn (part axis on Z, X towards ceiling, Y back of machine) but it doesn't look like Mastercam handles it that way.  Any thoughts?  Good to be back

[crazy^millman]

3 minutes ago, Bob W. said:

I have a call in but haven't heard back yet.  Right now I'm just trying to get usable code with the upper turret.  I have done extensive programming of 4 and 5-axis machines so the indexing aspect should be pretty straightforward.  What WCS should I use for setting up my parts?  For my HMCs I have always set the parts up as the machine is and created planes for B-axis indexes as opposed to setting it up to use Mastercam's right and left planes for 90 degree indexes.  I would like to do the same for mill-turn (part axis on Z, X towards ceiling, Y back of machine) but it doesn't look like Mastercam handles it that way.  Any thoughts?  Good to be back

In MT they like for you to use the Create Milling planes process for your planes. Then when you grab them in the operation you're good. You can make planes like you are use to and use them for indexing. The BASE WCS is set when you do the job setup. Then you work from there.

[JParis]

Bob,

To get into the control def...load the machine and setup a part, toolpath or 2...keep it simple for speed...

Now you should be able to get into Machine >> Control Defintion       Wrong module open, sorry

As far as setting up your part...WYSIWYG   so set up the part as it will actually sit in the real world machine...no real flexibility there

 

Control def access is in Codemeter...When you hit G1 it will load the IOF file into Codemeter...

in there go to Home >> NC Configuration....what's end user available is in there

[crazy^millman]

You can use the control definition to build your holders and tooling if you want for your lower turret if you got one. I strongly recommend using the 3D tools.

Did you get an CAPTO, HST or CAT Spindle? Lower Turret?

[Bob W.]

In the job setup the WCS is set tp 'Top' but that has Z pointing toward the ceiling, 90 degrees off from the part axis.  The stock and jaws are shown along the X-axis of the Top plane as well.  It is a little confusing.  The plane that reflects the correct orientation of the part, stock, and jaws was created by Mastercam along with 6-8 additional planes.  This plane is:

DMG Mori Seiki NTX2000 1500SZM - Gen 1, which is the second plane created after DMG Mori Seiki NTX2000 1500SZM - Gen WCS.  The Gen WCS matches the orientation of the Top plane but is in a different location by several inches.  It looks like Mastercam is trying to do a lot to mimic the machine's coordinate system locations and I'm not sure I'm crazy about that.

20k Capto C6.  Using Sandvik Capto C4 quick change on the lower turret.

[JParis]

5 minutes ago, Bob W. said:

DMG Mori Seiki NTX2000 1500SZM - Gen 1, which is the second plane created after DMG Mori Seiki NTX2000 1500SZM - Gen WCS.  The Gen WCS matches the orientation of the Top plane but is in a different location by several inches.  It looks like Mastercam is trying to do a lot to mimic the machine's coordinate system locations and I'm not sure I'm crazy about that.

As you go through the set up, which you MUST do first, it will all fall into the correct positions.

The workflow in MT vs standalone MCAM is definitely different...it does work but it's different

Left spindle on the origin, the right spindle is created automagically going through the Job Setup

[Bob W.]

12 station lower turret with 12k live tooling and y-axis

John, how much programming have you done in MT?  How do you like it?  What machines are you programming with it?

 

[JParis]

9 minutes ago, Bob W. said:

John, how much programming have you done in MT?  How do you like it?  What machines are you programming with it?

 

A fair bit Bob, though I'd like to spend more time in it but our call for complex parts that require offline programming isn't a heavy burden. I am currently the only one here that can run it.

I like it for the most part...I was involved very early on before it was released so I had a familiarity with when I landed in this position. We have Mazak Integrex's

[Bob W.]

11 minutes ago, JParis said:

As you go through the set up, which you MUST do first, it will all fall into the correct positions.

The workflow in MT vs standalone MCAM is definitely different...it does work but it's different

Left spindle on the origin, the right spindle is created automagically going through the Job Setup

 

Right, but when I initially import the part I plan to program, where do I put it?  If I orient the part relative to the 'Top' plane with the part axis aligned to the Top plane's Z-axis it doesn't go well.  If I align the part to the Top plane's X-axis it works much better.  It appears that I shouldn't align the part to the Top plane coordinates as it would go into the machine.

[crazy^millman]

The machine environment it completely different like John said. However once you get get into the swing of things you will be able to wrap your head around it.

[Bob W.]

2 minutes ago, crazy^millman said:

The machine environment it completely different like John said. However once you get get into the swing of things you will be able to wrap your head around it.

Right, just trying to get over the initial learning curve.  Where do I find the post?

[JParis]

Assuming your standard XYZ WCS as a base...

The X+ direction will be your Z0 face....Y+ will be your back plane...Z+ is looking straight down from above....

I place my centered on the origin hairs, then I transform it X- so the right face is on the origin.

1 minute ago, Bob W. said:

Where do I find the post?

It's part of the .machine file but it is not available for editing to the end user

C:\Users\Public\Documents\Shared Mastercam 2021\Mill Turn\machines

[Bob W.]

1 minute ago, JParis said:

Assuming your standard XYZ WCS as a base...

The X+ direction will be your Z0 face....Y+ will be your back plane...Z+ is looking straight down from above....

I place my centered on the origin hairs, then I transform it X- so the right face is on the origin.

Perfect, that is what I arrived at to make it work.  It is a little frustrating but I'll get used to it I guess.  I assume I will not program from the Top plane, I will use the planes the job setup created?

 

[crazy^millman]

4 minutes ago, Bob W. said:

Right, just trying to get over the initial learning curve.  Where do I find the post?

They are using MP.NET and the post is not accessible to the end user.

[JParis]

Just now, Bob W. said:

Perfect, that is what I arrived at to make it work.  It is a little frustrating but I'll get used to it I guess.  I assume I will not program from the Top plane, I will use the planes the job setup created?

 

For your turning yes...for milling you will make your planes...

[Bob W.]

1 minute ago, JParis said:

For your turning yes...for milling you will make your planes...

When I make my milling planes, which do I use as the WCS?

When programming for indexing...

[JParis]

4 minutes ago, Bob W. said:

When I make my milling planes, which do I use as the WCS?

When programming for indexing...

That's another place it functions a little different, you have this going on..

It will select your spindle origin and then let you apply the correct plane for what you're trying to do

[Bob W.]

5 minutes ago, crazy^millman said:

They are using MP.NET and the post is not accessible to the end user.

Where would I make the changes for tooling output?

[Chally72]

Do you guys also use the Align to Z command along with the "Transform to plane" setting? This is how I orient MT/Lathe parts correctly before starting Job Setup/programming

 

 

[JParis]

1 minute ago, Chally72 said:

Do you guys also use the Align to Z command along with the "Translate to plane" setting? This is how I orient MT/Lathe parts correctly before starting Job Setup/programming

 

 

I haven't had to as yet...most everything comes in with a standard orientation, I just transform it where it needs to go...that is something I should try and remember though