New to 4th axis-- any tips for a n0ob?

[jeff]

I a few days we are getting a new Okuma VMC with a Tsudakoma rotary, this machine will mainly be running shafts with a tailstock doing keyways and cross holes,other work that requires 4th axis stuff,and of course vise work.

For someone that has never programmed or rana full 4th rotary, are there any tips you pros can give me?

Thanks!

[jeff]

Nobody had any Do's or Don'ts?

I'm getting the turorial cd soon, but I just wanted to get a headstart.

 

What about my post... stuff like this:

 

rot_ccw_pos : 1 #Axis signed dir, 0 = CW positive, 1 = CCW positive

index : 0 #Use index positioning, 0 = Full Rotary, 1 = Index only

ctable : 5 #Degrees for each index step with indexing spindle

use_frinv : 1 #Use Inverse Time Feedrates in 4 Axis, (0 = no, 1 = yes)

maxfrdeg : 2000 #Limit for feed in deg/min

maxfrinv : 999.99#Limit for feed inverse time

frc_cinit : 1 #Force C axis reset at toolchange

ctol : 225 #Tolerance in deg. before rev flag changes

ixtol : 0.01 #Tolerance in deg. for index error

frdegstp : 10 #Step limit for rotary feed in deg/min

 

Do I always want inverse time?

[Jayson Kramer]

I like tp program from Z zero to make life easier on center of rotation.

[Guest]

Impossible to say on the Inverse feed, that will be determined by your machine, not Mastercam, most of your post settings will be driven by what your control requires as well, so going through the post now, tough to say

 

As Jay said, I prefer to program for centerline of rotation

[Newbeeee™]

Jeff,

For round work or more open limit, we'll program Z centreline of rotation with the 1x G54 datum.

Bear in mind that if you're using fixtures, no matter how good they repeat onto your 4th, they'll never be spot on so then...

 

If the part is more involved and we need to tweak datums or if we're using a vice, we'll use a G# per face. This is where mcam works really well imo.

So if you see a couple of pics attached I'll try to explain what we do. This is a poor mans hori setup

 

If you look at 4th axis setup.

Firstly rotate/move your part to get the correct orientation so TOP is as per the 4th axis, and the rotations (A90/A270) are correct to your views/machine.

Just use the one WCS for the whole setup, but a separate T/C plane for A90 and A270.

This hopefully explains the vice set ups:- We would use G54 datum for face 1 (top) with X & Y c/l of 4th axis, and Z would be 3.5mm up from the bottom of the billet. This is because the vice jaws are 3mm deep, and the centreline of rotation is 3.5mm 'up' from the billet base.

A270 would be G55 with X&Y c'l of 4th axis, and Z would be the top of the skimmed face. So any Z cuts would now be minus (ie into the part). This works better for clearance on index moves - put a Z ref position in the last toolpath just before the index move so the tool can get high enough, and all your other clearances can be snug to the G55 face.

To get the Z zero to be the machined face, in mcam view manager, click on the Origin (View Coordinates) Z value and all will be clear.

A90 is a repeat of the above, except it is G56.

 

To do the other 3 sides, create your new TOP view by solid face (or whatever means) and save this. Note that when creating, the XYZ directions need to be in the correct orientation so your following A270 and A90 views will be correct.

Assign a new WCS and use the Origin to set the datums for your new view (X, Y and Z).

This would be G57 and because you have a new WCS, this *should* output A0.

Repeat as per above to create your new views, assigning A270 G58 and A90 G59.

 

Now it must be said that mcam view manager took a while (well quite a while actually) to get my head around. When toolpathing, be careful that you are always in WCS1 for the 1st 3x ops and WCS2 for the 2nd 3x ops.

You can add a comment to the view manager (in lieu of not being able to rename the views) for WCS1, and for your new views, you can name them WCS2 A0 TOP and WCS2 A270 for instance.

We also disabled the -1 automatic work offset numbering system in our post. To me this is soooooooo dangerous having this feature (especially when I don't know what I'm doing!) so we enter in the number as we want it, and the post outputs exactly what we want.

 

Lastly, it's worth configuring X+ so you can oneclick it and up comes the ops with the G# showing, just to double check all is correct. It's saved me lots of times when learning, as a wrong G# number is the easiest way to wreck a machine (hence the stupidity of automatic G# numbering imo).

Hope this helps

[Rstewart]

Good write up Newbeeee.

 

Also a lot of times you can just get away with drawing the part in MC how it sets in the machine and use one offset. X,Y,Z, offsets at centerline let MC do the rest. Lots of different ways to skin a cat...

 

Tons of people on here much smarter than I, Still learn new stuff errday on here

[jeff]

Awesome tips, thanks everyone!

[Chris Rizzo]

Invest in a Big Kaiser or Shunk Unilock system for your fourth. Make some tombstones, you can approach horizontal w/ pallet changer spindle optimization.

 

We also disabled the -1 automatic work offset numbering system in our post. To me this is soooooooo dangerous having this feature (especially when I don't know what I'm doing!) so we enter in the number as we want it, and the post outputs exactly what we want.

 

Big time be aware of that. Alternately, just make sure you have a value entered in your view manager for each and every view. Even if you want G54, don't leave it empty, have a 0 in there. Multiple views have the same offset, have the same number in the woff field in view manager.

 

Another tip is set up the icon G view = T plane. That way with one click you can visually be looking down the spindle and be sure your on the view you think you're on.

[Newbeeee™]

Thanks Chris for the tips.

We modded our post so we can actually enter 54, 55, 56, 57, 58, 59 and it throws an error when posting if anything else is entered.

Yes I know this only works with fanucs, but that's all we have, and doing this, what we want is what we get!

I've never had to use it yet, but I've been thinking about extended offsets and mod the post again so we can enter 541 for 54.1, 542 for 54.2 etc. Came close to needing it on one job but got away with not needeing it in the end

[Newbeeee™]

 

Another tip is set up the icon G view = T plane. That way with one click you can visually be looking down the spindle and be sure your on the view you think you're on.

Just added this to the toolbar - I like this a lot