4th Axis rotary positioning with one offset - cant seem to get it

[Inthebayy]

Hey guys,

 

Firstly, yes, I have searched the forums and tried many different ways to get this to work, and I feel I'm just missing something simple that's affecting the whole process.

 

Machine is a Haas EC400.

 

I have a 5" tombstone with 4 parts on it, two per face on opposing sides, B0. and B180. The parts need to be hit from their relative front face (0deg) and both sides (90 and 270). I've programmed the part with the top plane at the center of the tombstone, and each part also has its own offset for their B0. center and top surface.

 

 

For instance, G55 is set at 2" from the top of the base of the tombstone, and the center of the tombstone, and G54 is the center of the bore that you see that has the toolpaths associated with it, with Z set at the furthest point from the tombstone.

 

G55 = Top

G54 = Part Probed origin

 

I have the WCS for all operations set to TOP.

I have the T/C plate for all operations set to their respective planes that I have created off of the geometry from the part. This was done by dynamically rotating the G54 plane to be oriented correctly, so the centerpoint is still as-described for G54, just reoriented.

 

Those rotational planes have their work offset set to G55, is this correct? Should it be G54, even though the WCS is still for TOP?

 

 

When I try to run the code, it trips a limit or otherwise does not drill where I want it to. Should I be using the right/left planes that already exist? Should the side planes be set to G54 (the probed part offset) or otherwise? Does anything stand out? Because right now I'm just lost for what to do.

 

Thanks!

 

[Brian Pallas]

I would use a work offset for each station.  Then use G10 to write the offsets in.  That way it is still a fast setup without needing to set a XYZ for each station, but each station can still be adjusted if need be by the operator.  Set the work offset for each view in the view manager.

[Inthebayy]

I would use a work offset for each station.  Then use G10 to write the offsets in.  That way it is still a fast setup without needing to set a XYZ for each station, but each station can still be adjusted if need be by the operator.  Set the work offset for each view in the view manager.

Yes, that's a good way to do it, but you seemed to miss the point of my question, in that I can't get it to rotate correctly.

[Thee Awbade™]

Yes, that's a good way to do it, but you seemed to miss the point of my question, in that I can't get it to rotate correctly.

 

Are you certain that it's the program? Is your rotary table proven to be accurate and working? 

[Inthebayy]

Are you certain that it's the program? Is your rotary table proven to be accurate and working? 

Its definitely functioning. If it wasn't I wouldn't be here. It does run other programs successfully, although I have yet to program with this style of one-origin programming.

[crazy^millman]

Okay so they all share the same Origin which is COR programming. The planes would be the same as Left or Right Plane for the B90 and B270 is Front was your B0 with respects to a TOP WCS. A quick test would be take the B90 and B270 operations and just edit them to use the Left for the plane that correct one and then Right for the plane that is correct. If that works then that tells you the planes you create were not created correctly.

 

The resident expert on HMC programming should be chiming in an minutes and he will get you all sorted out.

[Sticky]

If I understand this correctly, G55 is your center of rotation, and G54 is the center of the bore of one of your parts?

 

Mastercam will not automatically calculate your work offsets for you. You will either need to modify your post to do this for you, or you will need to calculate them yourself and enter them in the control by hand or use a G10 in the top of your program. It doesn't really sound like you have decided if you are going to program off center of rotation only, or use work offsets. Being that it looks like you are probing and working with predefined shapes, I'd use work offsets.

 

Which means that your parts would have 3 offsets, ie G54 for your bore, G55 for the right side, G56 for the left side.

 

 

[Inthebayy]

Hmmm, okay. I'll play around and see what my local support has to input on the matter and post what I come to. Thanks all for the information.

[Colin Gilchrist]

I think you are getting some things confused in how you setup your Planes for a Horizontal machine. For programming a Horizontal machine, most post processors are setup to use "Top" as the WCS, and "Front" as the Plane orientation for B0. on the tombstone. The Work Offset number is set with the "work offset" value in the planes dialog. You can set this in the operation, but I prefer to set my Work Offset number value in the Planes Manager. This gives you the ability to associate a Work Offset number with a specific Plane being used.

 

The NC code in Mastercam is always output relative to the "Origin" of each Tool Plane. With the setup you have shown in your picture, if that picture is taken in an Isometric view, then your parts are not setup correctly according to the picture you are showing. That picture shows parts on the Right and Left Plane orientation. That would give you "B90." and "B270." if you programmed the "face" of that part. (the axis of the bolts holding the part to the face of the tombstone is what I'm referring to.)

 

So, assuming your parts are mounted correctly, using the Front and Back Planes, you are going to need to decide where you want the origin of the NC code to come from. Start by creating a "Point" entity at the Center of Rotation. If you look at the tombstone/parts from the Front view, you are looking straight through the spindle of your Horizontal, facing the parts. X+ points to the right, and Y+ starts at the bottom of the tombstone, and goes vertically towards the top.

 

Now, you have four parts on your tombstone. It looks like each part has work that is done from three sides. I would recommend using three Work Offsets per part position. That gives you the ability to make adjustments to each part individually.

 

Let's assume that the large bore/pocket is facing you in the Front plane. I would use "G54" for the part near the Top of the Tombstone, and "G55" for the part near the bottom. Since both parts are on the "Front" Plane, but use different Work Offsets values, I would take the "Front" plane, and make 2 copies of it. Rename the first copy "FRONT - PART1 - G54", and set the Work Offset value to '0'. Then name the 2nd copy "FRONT - PART2 - G55", and set the work Offset to '2'.

 

Now, you can set the "origin" of each of these planes to whatever surface/feature you are going to "dial in" at the machine. This could potentially be the Center of rotation, but that means you have to draw up your part/fixture exactly in the correct place, relative to those incremental values on the machine. Otherwise, you can use the "origin" XYZ data entry fields (or better yet, have a "point" entity on a separate level, in the correct spot, and use the "select" arrow to pick it.) That sets the location from where your NC code (on using that tool plane) will come from.

 

Now, go to the "Right Plane". The tombstone would be rotated to B90., but now you've got to make operations on 4 parts. Two on the left side (Parts 1 and 2), and two on the right side (Parts 3 and 4) in this "view".

 

I would make 4 copies of the Right Plane, and name them "PART # - RIGHT - G5X". (change the part # and work ofs value), and set the Work Offsets to '2', '3', '4', and '5'. That gives you G54-G59. (Assume when looking from the RIGHT plane, that top left is Part 1, bottom left is Part 2, top right is Part 3, and bottom right is Part 4)

 

For each of these copied planes, set the Work Offset Origin accordingly. Every time you pick a new Tool Plane Orientation, the origin values are relative to the XYZ axes of the Tool Plane. That means that these values change for each position you pick. (even though you might be picking the same "point", if the plane changes, so will the XYZ positions.)

 

OK, so on the "Back" side, B180., make two copies of Back. Rename them to use "G54.1 P1" for Part 3 (top part, on the back side), and G54.1 P2 (bottom part, back side) for Part 4. Set the origins using point entities on your parts. Set the Work Offset values to '6' (G54.1 P1) and '7' (G54.1 P2).

 

Last step is making 4 copies of the Left Plane. That would be B270, and Part 1 is top right, Part 2, bottom right, Part 3 top left, Part 4 bottom left, when looking at the LEFT plane. Use G54.1 P3 for Part 3 (top left), G54.1 P4 for Part 4 (bottom left). Use G54.1 P5 for Part 1 (top right), and G54.1 P6 for Part 2 (bottom right). The Work Offset values are '8', '9', '10', and '11' for those planes. Set the origins accordingly.

[Sticky]

Well explained Colin!

 

Inthebayy, just so you know you can have your post setup to automatically calculate your workoffsets and enter them in the header of your program. This makes for a very simple, reliable, and robust method of programming hmc's. It just so happens Colin could make those mods for you, I highly recommend them, and him!

[Inthebayy]

Wow, that was truly extensive Colin. (oddly, I have the same name, hooray for single L Colin's!)

 

I was hoping to be able to still include probing and work off the center of rotation, but it seems like Colin's way is the way to go. I've made a working copy and I'll give that a shot today and see how it goes, I don't expect any problems.

 

Thanks everyone for all the help, I'll report back later.

[guitar]

"I have a 5" tombstone with 4 parts on it, ..."

 

A picture is only worth 1000 words. An MC file s worth a million. Post your file here.

[Inthebayy]

"I have a 5" tombstone with 4 parts on it, ..."

 

A picture is only worth 1000 words. An MC file s worth a million. Post your file here.

I unfortunately am unable to post the file publicly, or I would, if you would like to take a look, PM me your email.

 

So I've created all the planes and made a separate group with a copy of my toolpaths. Now the problem I'm finding is that Mastercam is not posting my new work offsets per indexed face.

 

Example:

%O2000 (SEA103486)(SEA103486-1)(T2   - 1/4 SPOTDRILL        - H2   - D2   - D0.2500")G00 G17 G20 G40 G80 G90G91 G28 Z0.(CDRILL 4BOLT SIDE)N1 T2 M06 (1/4 SPOTDRILL)G00 G17 G90 G57 A-90. X0. Y1.25 S6000 M03G43 H2 Z7.5Z.18G94G99 G81 Z-.17 R.18 F10.G80Z.25X-.2972 Y.2972G99 G81 Z-.1 R.25 F10.X.2972Y-.2972X-.2972G80Z7.5(CDRILL FRONT)A0. X-.6669 Y1.8324                  <---- no work offset updateZ7.5Z-1.375G99 G81 Z-1.575 R-1.375 F10.G80X-1.23 Y1.375Z-3.G99 G81 Z-3.2 R-3. F10.G80Z-1.986X-1.5 Y.813G99 G81 Z-2.186 R-1.986 F10.G80X-.825 Y.845Z-3.G99 G81 Z-3.2 R-3. F10.X.825X1.23 Y1.375G80Z-1.986X1.5 Y.813G99 G81 Z-2.186 R-1.986 F10.X1.65 Y.187G80Z-1.375X1.8324 Y-.6669G99 G81 Z-1.575 R-1.375 F10.G80X.825 Y-1.5Z-3.G99 G81 Z-3.2 R-3. F10.X-.825G80Z-1.375X-1.8324 Y-.6669G99 G81 Z-1.575 R-1.375 F10.G80Z.1X-.34 Y-2.5373G99 G81 Z-.1 R.1 F10.X.34G80Z7.5(CDRILL 2PORT SIDE)A90. X0. Y0.                        <---- no work offset updateZ7.5Z.03G99 G81 Z-.17 R.03 F10.Y-1.5G80Z.1X1.2 Y-1.25G99 G81 Z-.1 R.1 F10.G80Z7.5M05G91 G28 Z0.G28 Y0. A0.G90M30%

And yes, they have offsets in the Plane manager

 

Hmmm.

[Leigh @ Kodiak]

Maybe I missed it, but what post are you using? MP master uses Miscellaneous integers to lock on first WCS. (Lock on First WCS [0=No,1=Yes])

[Inthebayy]

Hi Leigh (its Colin, BTW.) The post was created by In-House based on MPMaster. I hopped into the first operation and found that it had been flagged as 1. Just changed it to zero, and that's solved my offset update issue. Thanks!

[jlw™]

I guess I'm missing something too. I've done a significant amount of 4 sided tombstone work myself. If you're using C.O.R. why are you probing? To use C.O.R. on a tombstone you must have the spec sheet from the tombstone maker and program accordingly in mcam.

 

If you want to probe and use C.O.R. you can probe points on the tombstone for G54.4/G54.2 dynamic offsets which will calculate deviations for you. Or you probe each face for a unique offset (G54, G55, etc).

 

You can also probe one face of each part and use G68/G68.2 and let the control calculate rotations for you.

 

There's more than one way to split the wig but you gotta pick one.

 

I like G68.2 for 4 sided work because you can probe the center of every part for its offset then when it rotates the machine will calculate the same point when its rotated.

 

Are the parts located on the tombstone with locator pins or are they just bolted to it (this is how I would decide what to use)?

[Inthebayy]

I guess I'm missing something too. I've done a significant amount of 4 sided tombstone work myself. If you're using C.O.R. why are you probing? To use C.O.R. on a tombstone you must have the spec sheet from the tombstone maker and program accordingly in mcam.

 

If you want to probe and use C.O.R. you can probe points on the tombstone for G54.4/G54.2 dynamic offsets which will calculate deviations for you. Or you probe each face for a unique offset (G54, G55, etc).

 

You can also probe one face of each part and use G68/G68.2 and let the control calculate rotations for you.

 

There's more than one way to split the wig but you gotta pick one.

 

I like G68.2 for 4 sided work because you can probe the center of every part for its offset then when it rotates the machine will calculate the same point when its rotated.

 

Are the parts located on the tombstone with locator pins or are they just bolted to it (this is how I would decide what to use)?

They are located with locator pins and held down with swing clamps.

 

I was hoping to be able to use COR programming while having the bore probed and machined perfectly on center, even if that means its programmed separately.

[jlw™]

They are located with locator pins and held down with swing clamps.

 

I was hoping to be able to use COR programming while having the bore probed and machined perfectly on center, even if that means its programmed separately.

 

I would recommend using G68/G68.2 if your control supports it. In this case you would probe each bore and face once and have one unique offset per part. Then, the function of the G68 will account for center of rotation when rotated so you only have one offset for each part and you'd probe XYZ of each part. I would even take two points on each face at extreme X points to set rotary offset.

 

Worked well for me with multiple parts on a tombstone so far.

[Rocketmachinist]

I'm moving to a shop that has an ec-400 also. The people there have not really mastered how to program it. If anyone is willing to share a simple file that helps to explain the whole process would be awesome.

 

I would recommend using G68/G68.2 if your control supports it. In this case you would probe each bore and face once and have one unique offset per part. Then, the function of the G68 will account for center of rotation when rotated so you only have one offset for each part and you'd probe XYZ of each part. I would even take two points on each face at extreme X points to set rotary offset.

Worked well for me with multiple parts on a tombstone so far.

 

I don't thinks Haas uses 68 in the way that other controllers use it. I could be wrong, I am kinda in the dark when it comes to horizontal programming.