5 axis trunion table center of rotaion

[JOHNAKA]

Hello everyone

 

I have a vm3 machine with trunion table 210T I believe the model that embedded in mastercam when u load the machine configuration, it has the center of the pivots .125 above the top of the trunion table. I always kept the z0 inside mastercam on the distance center of the pivots. And I always placed the geometry part and fixture on the top of the table and counting the distance from the table top to the pieces. I been doing this for some time now. I got into some adjustments, like if I title the table 90 deg, we will have some .02 or shift on the y axis need to be adjust, so I called my reseller and they said to move z0 inside mastercam to the top of the table and put the shift axis in the post saxisz .125 claiming that should solve the problem. But that’s didn’t work, it made it worse, does anyone here using the same procedure, any help will be appreciated. Thanks

[crazy^millman]

Sorry, but they should have instructed you to look at the offset settings in the post and make sure those are correct first then have you make those types of adjustments. Basic setting up a 5 axis machine is to #1 figure out where the Pivot point is. Once that process is established then build the test process from that. Basic 5 axis block test should be good enough to run it through everything you would need.

 

Make a test block where you cut 5 side of a block in the standard views. Then do simple 5 axis test cuts on a sphere to make sure the tool will contact the sphere where you need running through all possible travels as part of that test. Once you have all of that dialed in then do 5 axis drilling in 20 to 30 different index locations. I have been working on making up a sample test piece to use for testing posts. As soon as I get it perfected I will be posting about it on my new blog I am starting up.

 

Basic test make a 3 inch cube. Take a cut on each of the faces, but do not do it 3+2 do them as 5 axis cut from Mastercam. Yes technically they are 3+2 when you toolpath them, but that will give you some good information. From there you will know what is going on to then make the adjustments needed to either your programming or to the post to adjust for the problems you are seeing.

In the post you will need to look here:

 

#Axis shift
shft_misc_r : 0	 #Read the axis shifts from the misc. reals
#Part programmed where machine zero location is WCS origin-
#Applied to spindle direction, independent of RA
#Table/Table -
#Offset of tables to secondary axis relative to machine base.
#Tilt Head/Table - Head/Head -
#Part programmed at machine zero location-
#Offset in head based on secondary axis relative to machine base.
#Normally use the tool length for the offset in the tool direction
saxisx	 : 0	 #The axis offset direction?
saxisy	 : 0	 #The axis offset direction?
saxisz	 : 0	 #The axis offset direction?
r_intersect : 0	 #Rotary axis intersect on their center of rotations
				 #Determines if the zero point shifts relative to zero
				 #or rotation with axis offset.
#Nutating axis shift, used when calculations are based on mtype 3 or greater
#'top_map' and toolplane tool paths use the axis shifts above, 5 axis use these
n_saxisx	 : 0	 #The axis offset direction?
n_saxisy	 : 0	 #The axis offset direction?
n_saxisz	 : 0	 #The axis offset direction?
n_r_intrsct : 0	 #Rotary axis intersection with nutating (normally zero)

 

Once you figure out what the offset needs to be then you should be able to program from Zero in Mastercam and have the machine follow that same process from the posted code. No reason you should be programming they way you have been. Mastercam has everything you need to get good code on that machine, just need to adjust your post to make it happen.

[CJep]

John the reason for doing the shift in the post would be if the center of rotation for the A & B did not intersect,....

 

If you're not familiar with finding center of rotation, Karlo Apro's book "Secrets of 5axis Machining" has a detailed guide to find the rotary zero position.

 

If you are using the Generic Haas TR post that is installed with Mcam,....

I will use Mcam's origin as the center of rotation, then set the part up in Mcam relative to it's fixture location in the machine. All the toolplanes I use to position the part will use Mcam's origin as the center of rotation.

[JOHNAKA]

prisme

 

i do have the procedure for finding the center of rotation on the trunion, by using 123 blocks it is exactly .1248, and i do the programming on what u explained. but yet there still some shifts i need to align either goemtry or offeset on the machine. for example i was cutting a titanium fan the vanes depth 1.5 so i did it in 3 depth, .5 as it goes around and finish that, the next depth is 1 and goes around and finish that the last depth is 1.5 and goes around and finsih. well here is the big problems

there were mis matches with .5 to 1. depth with 1. deg ratoted geo to fix., and between 1. to 1.5 almost 2 deg rotated geo to fix, i know there must be some blades deflection but i dont believe it is that much, simulate that in mastercam before u do the adjustment and u dont see any mis match at all. of course u will need to reck a part to see that.

[CJep]

page 22 in the pdf:

 

http://www.modulewor...0 Optimized.pdf

 

Are you saying that by your measurements you found the intersection of the A&B rotary to be off by 0.1248?

 

But also you should take a look at what Ron "Millman" described as well setting up a 5 axis block test would be better than scrapping a part going for the money shot.

 

CJep

[mkd]

he is saying that on all Haas 5ax trunnions the A axis center of rotation is .125 above/away from faceplate.

 

what he is doing with offsets and why; i have no clue. he should only need ONE offset for all angular positions.

[CJep]

The .125 center of rotation above the face plate is not so much of a problem, you will need to allow for that in the fixture location in Mcam, you need to know what the fixture location distance is to the center of rotation, then Mcam's origin can be used as the center of rotation for the multiaxis toolpath.

 

If the relation of the center of rotation for the A axis does not intersect the B axis rotation then that offset needs to be set in the post, as Ron stated but without verifying that offset it's like drilling holes in the bottom of the boat to let the water out.

[JOHNAKA]

PRISM

i do all that, i will post a picture hold on

[JOHNAKA]

The reseller want me to move the table solid up .125 and put that in the post. the question is does anyone done this.?

[bet338]

This is what I have in my post. As you can see the only shift is in the "Z" axis. Never did understand why Haas couldn't put their "A" axis on center of rotation.

 

 

#Axis shift
shft_misc_r : 0	 #Read the axis shifts from the misc. reals
#Part programmed where machine zero location is WCS origin-
#Applied to spindle direction, independent of RA
#Table/Table -
#Offset of tables to secondary axis relative to machine base.
#Tilt Head/Table - Head/Head -
#Part programmed at machine zero location-
#Offset in head based on secondary axis relative to machine base.
#Normally use the tool length for the offset in the tool direction
saxisx	 : 0	 #The axis offset direction?
saxisy	 : 0	 #The axis offset direction?
saxisz	 : 0	 #The axis offset direction?
r_intersect : 0	 #Rotary axis intersect on their center of rotations
				 #Determines if the zero point shifts relative to zero
				 #or rotation with axis offset.
#Nutating axis shift, used when calculations are based on mtype 3 or greater
#'top_map' and toolplane tool paths use the axis shifts above, 5 axis use these
n_saxisx	 : 0	 #The axis offset direction?
n_saxisy	 : 0	 #The axis offset direction?
[color=#ff0000]n_saxisz	 :.121    #The axis offset direction?[/color]
n_r_intrsct  : 0	 #Rotary axis intersection with nutating (normally zero)

[JOHNAKA]

bet338

 

thats great, thats what im looking for. did u move the table to .121 in mastercam to level up that with the post.?

[bet338]

Johnaka

 

Yes. We also have a stevens plate on it and we shimed it up .121, and still had to put .121 in the post. Now the stevens plate measures 1.250 so when I place my solid in mastercam the botttom of the part is at 1.250 plus whatever fixturing i might be using.

[mkd]

The reseller want me to move the table solid up .125 and put that in the post. the question is does anyone done this.?

no.

like Cjep says, put your part in mastercam in the same position it is in on the machine in relation to center of rotations, and forget these post-setting-offsets.

 

A/B axis intersect well (under .001") on Haas trunnions.

[crazy^millman]

bet33 thank what I was talking about put that shift in there leave the part on Zero run a couple testst cuts to make sure that did what you want and you are done. On other machiens we do this, but on this that is such a smaller difference then you let the post do all the thinking and work for you without having to always remeber to put the part in the postion it needs to be. Gcode taught me a trick years ago where using a point and setting your WCS off of that gives you tons of flexability when doing 5 axis work.

 

HTH

[Guest]

I have not seen many builders put their tables at the CL of rotations. Really it's irrelevant. Just model the everything as it sits in machine space and be done with it.

 

When I set up a new 5-Axis machine, I always run a test piece to get my true CL rotation positions and adjust until the part is .0001 or better positionally. Sometimes it's .00009 but I can't split .0001 so it is what it is. If I were running the machine in metric mode, I could get it within a micron but I digress.

 

Usually my test piece is a block. I'll interpolate a hole halfway through plus any radius, then rotate 180 and do the same. I'll get those two holes to match up which takes care of X and Y, then I'll face it on 2 sides to handle Z. That's worked for me.

[Bob W.]

Here is how I set up my trunnion (Haas TR160). First I put an indicator in the bore and rotated the B-axis 360 degrees to verify that the bore is true with respect to its axis of rotation, which it was. When installing the trunnion I probe that bore for X and Y, making sure the A-axis is at A0.0 (or perfectly horizontal) when doing so. I then set the A-axis grid offset so that A0.0 corresponds to the home position. I did this once a long time ago so I don't recall exactly what I did but it was a parameter setting. I do verify it every so often though to make sure there isn't any wander or shift. I then jogged the a-axis to A90.0 and probe the surface of the plate in Y and record the value. Next I jog the a-axis to A-90.0 and probe the surface in -Y and record the value. Half the difference between these two values is how high above the plate the A axis of rotation is. In my case it is 0.1285". I only ran through this procedure once when I received the trunnion but I do verify the measurements periodically.

 

One thing to note, my trunnion's b-axis plate isn't even flat. It is dished by .0005" (low in the center) so I always make it a point to probe Z in the same distance from the center along the x-axis. I doubt you will hold better than .001" on a Haas trunnion given that the plate parts and fixtures are mounted to is out of flat by .0005" LOL... It is pretty handy though, I'll admit that.

[crazy^millman]

Bob the best way and only accurate way to know 100% what is it.

[Guest MTB Technical Services]

Point of clarification.

The A-Axis rotates about a centerline parallel to the X-axis and the B-Axis rotates about a centerline parallel to the Z or Y depending upon your home position setup.

The centerlines of the A & B rotation on the TR-160 and TR-210 do indeed intersect according to the drawings from Haas.

 

TR-160

http://www.haascnc.c...ine Views_B.pdf

 

TR-210

http://www.haascnc.c...chine Views.pdf

 

The platter surface, however, is shown to be nominally 0.125" below the A-Axis centerline and parallel to the XY plane.

This surface has absolutely nothing to do with the center of rotation.

It is simply a necessary reference value for positioning your fixturing and workpiece in Mastercam relative to the main WCS.

The WCS Origin in Mastercam and Center of Rotation on the machine should be the same point.

The patter in Mastercam should be the same 0.125 nominal distance from the centerline of A-Axis rotation or Z-0.125

 

As long as the centerlines of rotation actually intersect, getting the post to give your correct output is easy.

Where it gets dicey is when the centerlines of rotation DON'T intersect.

More trig for the post involved there.

By this I mean the unit is designed this way.

I don't mean the deviation that shows up when you actually indicate your trunnion.

 

Just didn't want there to be confusion about what center of rotation actually means.

 

Here's a short sample that some of my students did.

 

The same principles apply.

The centerlines of rotation intersect and the work is positioned in Mastercam accordingly.

 

Your accuracy will only be as good as the least accurate part of the setup.

[JOHNAKA]

happy 4th of july everyone. hope you all had a good long weekend,

MTB

I place geomtry in mcx exactly like the part on the machine, wcs on hass (G54 Z0) is on that .125 above the table. so is wcs in mastercam. so what you saying is put the part exactly like on machine in mcx and forget the post shift.?

[Guest]

Having your part in Mastercam as it is in the machine is the best way to get what you expect.

[gcode]

Here's a quick way to check your setup.

I do this on all 5X files just to give the operators an easy eyeball way to

check their setup and my NC file.

Spot check a hole pattern on the stock with a 3X drill cycle.

Then spot check the same spots with a 5X ( or 3+2) drill cycle with the table ( or head) at an angle.

If the tool doesn't go to the same spots for both tool paths.. something is wrong.

[Guest MTB Technical Services]

happy 4th of july everyone. hope you all had a good long weekend,

MTB

I place geomtry in mcx exactly like the part on the machine, wcs on hass (G54 Z0) is on that .125 above the table. so is wcs in mastercam. so what you saying is put the part exactly like on machine in mcx and forget the post shift.?

 

Yes.

 

As James said, having your part in Mastercam as it is in the machine is the best way to get what you expect.

 

You should only use the post shift if the actual deviation from true center of rotation keeps you from making your parts within the tolerance required.

As long as you indicate your center of rotation within a few tenths (x.xxxx) and set your G54 Origin ( X0,Y0, Z0 ) from that, you really shouldn't have a problem.

Your Mastercam WCS should be your G54 Origin ( X0,Y0, Z0 )

 

If you do have issues it means your setup doesn't match what you actually have in Mastercam.

Double-check ALL fixture dimensions and locations once mounted to the platter.

 

I would use G-Code's testing method to verify your setup is good.