5-axis setup (BUDGIE)

[DavidB]

I have a Rotary table that goes into our Horizontal Makino.

My post rotation point is the centre of the B- axis and the centre of the rotary axis which is in the X-axis.

 

That means my G54 is centre of roation.

 

Is it possible to set a different work co-ordinate on the Machine say off a pre machined feature but still program the part in MC about the rotation points?

 

Or is the G54 fixed to the rotation point?

[Bruce Caulley]

Does your makino have an offset page with G54.1 G55.1 etc? If so you can use dynamic compensation and do exactly what you want. If not then I don't think so.

 

On our 5 axis mazaks we have this feature and leave the G54-G59 as 0,0,0,0,0

 

The Datum on the workpiece is set via the G54.1 page and the control uses the difference between G54 and G54.1 to automatically compensate. In MC the WCS origin for that op and all the toolplanes in that op is the workpiece datum in the machine. The operator can set the job up anywhere on the table or pallet and it doesn't matter.

 

HTH

 

 

Bruce

[DavidB]

Thanks for the reply Bruce.

 

 

That sound exactly what I'm looking for. How can I tell if the machine has this G54.1 function.

 

quote:

---

In MC the WCS origin for that op and all the toolplanes in that op is the workpiece datum in the machine.

---

Wouldn't the Origin in MC stay as the rotation point of the axis's for the post and then the machine G54.1 can be set anywhere and the controller caculate the differances?

 

 

[Jack Neelands™]

Howdy Dave... i posted a string in here for cnjb on some tomestone programming that does this ... zipped for ya to look at in the X folder...zipped file is called S00B04D.prt.zip and has 4 examples of hydraulic manifolds programmed with the tombstone as the center but allow for offsets to be changed...just make all the coordinates the same in the machine and move if necessary...ie g54.1 to g54.12 are all the same but g54.13 needs a few thou up for some reason or in some other location on a vice that had to be moved...this allows the operator freedom to move the parts around or leave it in center of table...mind you if you have to use a particlur datum on a part then you will have to move it to that location and force the post to output the new work coordinate

[Rick Henrickson 65]

David they are in your work offset page same as your G54 just page down a few then you should see them If you have the option

[Post dept]

David,

 

The datum track feature would be killer for you. Makes part setup so much easier.

 

If not available, you could try the following as an alternative.

 

Setup your part on the machine, probe for the features you want to pick up. Add that B-axis value to your datum. In mcam, output your toolpaths with respect to those datum points using that toolplane as your WCS. So, you're effectively getting code output that is consistent with your backplot (with respect to that plane). When you call G54 B0, your part indexes, and the code comes out in that spot.

 

You can even get your post to do a G10 parameter load that will tell the machine that G55 position in coodinates with the angular component. Kind of like getting the post to do your 3+2 datum tracking for you.

 

That's the best way to work with off-centre datums if you don't have the datum track.

 

Slightly tougher to program in mcam, way easier to setup on the machine.

 

Brett

[Greg Williams]

David,

 

Sounds like your talking about a dynamic rotation reature?

 

I have not seen a Makino A55 with this.

 

You will need to follow Brett's advice above

[DavidB]

This is the setup..

 

How is it best done so I can clock the bore in this component as e ref and program in MC?

 

Budgie it,s a A66

[Bruce Caulley]

David,

If each part is different and you need to clock each one I don't think you will get away without either multiple datums or use Brett's method.

 

quote:

---

Wouldn't the Origin in MC stay as the rotation point of the axis's for the post and then the machine G54.1 can be set anywhere and the controller caculate the differances?

---

No, with dynamic comp you could set the datum as the top and centre of the bore in the part you have above. This would be the origin for your wcs and toolplanes in MC. When you set the datum in the control the machine compensates for the difference in your datum and the actual axis rotation points. I don't think your A66 will have this, but I might be wrong. Makino's controls are pretty basic even though the machines are $hi7 hot.

 

A cool example of this is if you use the rotary axis to cut a helix. With dynamic compensation the part doesn't even need to be set up in the middle of the table. The other axis will move to compensate as it goes around. This looks way cool if you ever need a demo for a customer to see.

 

Bruce

[Greg Williams]

David,

 

I do not see an easy solution to this one. As Bruce said you will need to clock each bore and then reference the position back to the CAD system and then move WCS.

 

Do you have many parts to do?

[DavidB]

So what your saying is unless I have dynamic compensation I would have to clock each parts bore then move the WCS in MC to suit regen, repost?

 

If so that's not an option.

[Bruce Caulley]

David,

Is there any way to fixture that will give you a repeatable location? Is this a casting?

[DavidB]

Parts are roughed and semi finished from a solid billet, Heat treated then finished machined. The Bore is the datum for all features the bore is Honed.

[Bruce Caulley]

If the bore is honed prior to this op can it be used as a fixturing datum?

[DavidB]

No there are still features in side the holed bore that need machining

[Bruce Caulley]

Bugger. What about some form of fixturing location that you can remove after final clamping? A block with a sliding pin that locates on the fixture somewhere?

[Post dept]

DavidB,

 

I just talked to Makino here. You can definitely purchase the datum track (Dynamic Fixtrue Offset) for your machine. It may be a hardware upgrade though.

 

Good luck.

 

Brett