Cancel
Showing results for 
Search instead for 
Did you mean: 

Okuma Multus Post Builder Milling Post. Coordinates transformation

Creator
Creator

Hello all!!!

 

I'm trying to do post for Okuma Multus B200 in NX Post Builder. This is mill-turn machine. As explained in tutorials about mill-turn posts I created two posts - one for lathe and second for milling operations.

With building lathe post i dont have serious problems yet but with milling part I got it.

 

I have one BIG quesion.

 

I need to mill pocket which has an angle with, for example X axis. On Multus X axis directed to top and coincides with direction of M-tool spindle (mill spindle), z-axis coinsides with lathe spindle, and y axis is perpendicular to both and directed to CNC operator.

 

In NX i have created cylynder in machine coordinate system. And created two milling operations. First for milling pocket in z-y plane so that the mill spindle directed by X axis. Second milling operation for creating pocket inclined at an angle in X-Y plane. When I do postprocessing NX give me coordinates and angles of tool tip in machine coordinate system (MCS).

 

Because in the first case direction of the mill spindle in NX MCS coincides with X direction of M-tool spindle of Multus i don't need to do coordinate transformation. But in second case I need. If, for example, in second case i need pocked inclined at an angle by 30 degrees from vertical X axis I can program in post for output G-code (M110 G138 C30) to rotate workpiece  by 30 degrees so that the pocket normal axis will be coinsided with X axis of okuma in reality. But wich MOM function i must to implement to convert raw output coordinates from NX MCS to Multus MCS i dont know.

 

Or maybe i need to implement for each mill operation its own MCS in NX and apply some MOM functions in post to go from one coordinate system to other?

21 REPLIES
Highlighted

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Esteemed Contributor
Esteemed Contributor

Typically the easiest way to do this (e.g Mazak Integrex machines w/G68 rotation) is (when the tool axis not parallel to MCS Z) to convert the post kinematics from a head-table post to a table-table post.  Rotate about the MCS zero.  Post then outputs "correct" XYZ positions automatically.  Including support for G2/G3 arcs, etc.

Only do this for "fixed" tool axis type operations (e.g. planar mill, face mill)

Drilling with mupltiple tool axes can also be handled (carefully!)

If doing full variable axis work, leave post kinematics alone & output the equivalent of G43.4?

 

There *might* be one of  the example machines/posts that does this, I haven't checked them out.

 

Hope this gives you some pointers...

 

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Creator
Creator
Thank you very much for such quick reply!Smiley Happy

I thought that in post builder exists some build-in MOM functions that performs this transformation, but I don't found them. Or maybe i don't understand some important basic things on CNC programming.

In reality on Multus there is exists G-code for coordinate transformation G303. (This code looks like PLANE SPATIAL on Sinumeric). The input parameters for this command is origin offset and three angles of new coordinate system. If I will create each mill operations in its own local MCS in NX I might apply this transformation for each operation on Multus but this is very uncomfortable because i will see one coordinates in program but machine will movie to others so it's easy to get confused. And in all cases I need to detect and calculate in post an angles for transformation from one operation MCS to other.

May you please give you answer in more detail?

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Esteemed Contributor
Esteemed Contributor

Yes, if you leave the kinematics as a "head-table" rotary axis setup, you (or more problematically, the users) have to remember to add separate MCSs for each "B" angle value, and then remember to put each operation under the correct MCS

 

That's the beauty of switching the kinematics to "head-head" rotary axes when you can - you just need the one (original) MCS in NX.

As the B axis changes, compute the G303 (or G68 or whatever) transformation (basically just the rotation angle of the B axis) & output it, rotating the machines CSYS around the NX MCS origin.

Not much need to calculate anything else - its "magic" :-)

 

Only big issues I mentioned in previous post - true 4/5 axis variable axis work, and drill cycles changing tool axis within an operation.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Creator
Creator
Hi Ken!

I will think about this.

But i have problen with programming rotation about C-axis. Not B axis.

Multus don't has table. It has Mill-tool (M-tool) spindle which can move in x,y,z directions and rotates about B axis which coincides with y axis. And it has C-axis - the axis of lathe spindle which is collinear with z axis of M-tool spindle. This is the axis of chuck for installing workpiece. You can 'google' the scheme of multus for viewing.

And I don't understand what simple MOM function transformation or G code I must use for side milling, that is milling at angle in x-y plane, or in other words if plane of mill pocket is rotated about C (or z) axis at some angle. I can manually rotate workpiece about C axis so that the plane where pocket will be milled will be located in y-z plane. But with this rotation I must do the coordinate transformation.

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom

Now we have postprocessors for Multus B300, B350, Macturn 250, Macturn 750, 2 channels, mill turn. With G137 contouring, drilling cycles, G158 5 axis, G255 5 axis.

Yes, for each 3+2 mill operation we rotated CSYS, and tool axis always along Z axis.

And we have CSE simulation models for Multus and Macturn.

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Esteemed Contributor
Esteemed Contributor

I have a Multus post working, so es, I know whata Multus (at least OUR Multus) looks like.

For C axis rotation, no need to have separate MCSs.

Just define the tool axis properly in the operation (perpendicular to floor or whatever).  The post takes care of rotating C.

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP5 + patch/TC11.2
I'd rather be e-steemed than e-diseaseled


Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Phenom
Phenom

I would agree with Ken's first post: with head rotaries - NX does not transform coordinates - with table ones it does. Using table/table to your advantage means even though you have a head type B and table C - you can still look at table/table for certain requirements (prismatic machinining with coordinate transformation.) Table/table also tells NX to put out circles in all planes.

NX10.03
Windows 7 Pro

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Creator
Creator
Thank you Ken!

I already solved my problem.
I just did not know that the post builder makes transformation by himself based on machine configuration selected in post builder. I never worked with CNC yet in my life. I thought that the coordinates that I see in "verify path dialog" in NX is the raw data and I must convert it by myself through rotation matrices in post builder, e.g. x1=x0*cos()+y0*sin() and so on.
But post builder rotates them by himself and give it to me in 'mom_pos' array!Smiley Happy I just need to use g-code to rotate about C axis at angle mom_pos(4)!
And I don't need to use various MCS, because with the knowledge of B and C angles I can do all in one global MCS.

But now I can not ever imagine situation in which i need to use several MCS. In what cases you use several different MCS?

Re: Okuma Multus Post Builder Milling Post. Coordinates transformation

Phenom
Phenom

If for some reason you want print dimensions and need X and Y to run a certain way - you may use csys type MCS to select the frame. This requires code in the post to make it happen with the frame applied (IE rot/trans or G68.) The coordinates you get will already be in frame.

NX10.03
Windows 7 Pro

Learn online





Solution Information