Rotary axis on machining centers

[nickz]

My question involves a "A" or "B" axis on vertical and horizontal machining centers. We are using Mastercam V8 (level 1). What is the most efficient way of programming the rotary axis. Presently we are creating the geometry at different view levels, utilizing a misc. real for degrees, and creating an operation for every single location. Is there a easier method? Is a higher level needed to make this easier?

[Guest CNC Apps Guy 1]

A = Rotary about/around the X Axis

B = Rotary about/around the Y Axis

The easiest way for ME is to draw it how it will sit on the machine. Change toolplanes as you need to index. Make sure you have your centerline of rotation correct, in a nutshell that's it. It's a tad more complicated than that but that's pretty much it. You can check it real easy in Backplot too. You can set it to make the part rotate and the tool will stay stationary.

Fun stuff, and it's more productive too. all the proper relationships are maintained between planes that way.

James Meyette

[Frank]

I do rotary machining all the time and James is right...what I have to use when rotating the geometry always use Cplane rotate. One question though how do you set up backplot and watch the part move ??

[nickz]

The geometry is 2D, and I can't rotate the part. For example, I have 2 different bores. Both will share X0, but different Y locations. I put them on different view levels so I can distinguish between the two, (usually there are a few dozen), create a drilling operation and input the degrees in a misc. real (mr9, post is modified to accept this). It's pretty much a flat drawing.

[Guest CNC Apps Guy 1]

Frank,

Go to Backplot. Set "Interpolate", "Animate" with "0" delay, ckeck "Simulate Axis Substitution" I usually use 1 Degree, then check "Simulate Rotary Axis", selct your tool orientation, and set the axis that you want it rotate about. That's it. Then run it. It really impresses people if you've got a lot of rotary motion. Shade your part, run it then walk away from your desk while it runs and see hom many people you have standing by your desk as it runs.

James Meyette

[d0gFartz]

James is right ....draw it the way it will be

fixtured......one thing that might save you

a ton of time is to use the named views,set

them up in your tplanes,if your gonna do

multiple ops like face,ctour,drill and such

on several parts take a cpl minutes and set

up your named views,that way you can just use

ALT+N hot key call em and set your t&c planes

right from there to work your way around your parts when you`ll be doin several ops,

also you can set up all your offsets right

from there and they`ll be in your tc planes

setting in your tool parameters page already

when you toolpath..i find that to be the best

way for me that way i dont gotta remember 12

or so offsets...since the whole idea behind

the horizontal is to save time and be able to

work on sides and angles and what ever else

on the part

[This message has been edited by d0gFartz (edited 01-23-2001).]

[Frank]

Hi Nick:

Maybe your just off to a bad start. Go to side view, set Z to 5.000, create a point at X0, Y0, now click on Cplane rotate, X+ and type 90. degrees, save. Change your Gview to the same number as your Cplane, create a point X0, Y0,. Now make sure your Tplane is also at the same number your Cplane is and do a drill cycle on your point, change all your planes to side, and do a drill cycle on the point you created at side. Now backplot. That example I use for horizontal machining, for vertical I use Top plane and rotate my Y + . Hope this helped. Also James I tried to backplot the way you described and it still didn't rotate the part.

Thanks

Frank

[email protected]

[nickz]

ok, need a chance to catch up. I completely understand that it needs to be drawn the same way it is going to be fixtured, but I need to understand one very important item. It should be drawn as 2D?, 3D wireframe?, solids?

What level of MC-Mill are you using? This has become very confusing. If anyone has a sample file for this situation, I would greatly appreciate the help.

[This message has been edited by nickz (edited 01-24-2001).]

[Frank]

Mill level 1 will do this it's just a 2d drawing on different planes. If you follow the steps I wrote above you will see how it works. You can still use levels for each rotary move or you don't have to.

Good Luck,

Frank

[Guest CNC Apps Guy 1]

Frank,

Do you have rotary motion in your code? If not it will not work. Go to side view, side construction plane. Create an arc 1.0 Dia. at Z0. Set your Z to -5.0. Now create another arc that is 3.0 Dia at the same center point as the other arc. Create 2 other arcs at the 0 deg. pos. and the 180 deg pos. at 1.0 Dia. Trim and fillet the three arcs together. Then go to isometric view while maintaining the side C/P. Create, Surface, Loft, pick one chain, then the other, make sure they(the chain arrows) run the same direction. Change C/P back to top. Then Toolpaths, Multi-Axis, Rotary 4 Axis. Pick the surface, select your tool, turn retract off and feed off as well (Only for illustrative purposes, I would never do that for real life stuff), then change direction to one way. Leave everythig else at the default. Once the toolpath calculates, filter it to .002 (it will speed the display up) Go to backplot and do what I said before and it will work.

James Meyette

[JoeyW]

James,

I tried following the steps you gave for getting the part to move in backplot but I still can't seem to get it to work. The tool rotates but my tombstone (and parts mounted on it) stay stationary. Is there something I'm missing?

[Kenneth Potter]

Chip Maker

I just tryed for the first time getting the tombstone to rotate to the z axis spindal"Side plane".From the tool path parameters box I set tool & cplane to each tomb stone face & set the rotary axis Rotation type to rotary axis positioning & rotate about z. Then set the back plot display simulate rotary axis to about z and tool orientation back .

Then back plot & watch the merry go round show ! Looks real kweul

Kenny

 

 

[Guest CNC Apps Guy 1]

Kenny, Way to go!

I like the show too. SOmetimes I'll just make something dumb to watch. I still get stoked when I see rotary axis stuff.

James Meyette

[Kenneth Potter]

James.

I learn the rotary axis learn stuff by studying the lathe c axis sample files.That got me started. E Z

Once i got it thru my thick skull, the difference between axis substiution & axis positioning, getting the tombstone to rotate during back plot issue became clearer.

Stayed up all night doing crazy things with tombstoning. I added multiple vises with parts loaded all over, Shaded every thing & got dizzy watching the backplot show.

The verify is still tool only rotation.

Can 8.1 verify rotate the rotary axis ?

Kenny

 

 

[This message has been edited by Kenneth Potter (edited 02-02-2001).]

[Guest CNC Apps Guy 1]

I have not tried it, but, I will venture to say....... NO!

James Meyette

 

[JoeyW]

Kenneth,

Thanks for the explaning it for me. i forget to turn on my axis rotation in the tool path parameters page. However, when I do turn the rotation axis on and set it to rotary axis positioning and rotate about z, when I go to regen the operation Mastercam crashed on me. Actually good old Dr. Watson pops up forcing me to crash. I've tryed this several times but with the same result. Help

MC V8.0 L1 running NT4 SP5

[This message has been edited by Chip Maker (edited 02-09-2001).]

[Kenneth Potter]

Chip Maker

IN the tool param,s page make sure your t&c planes & origins are the same.Hit F9 to see the system origin & tool plane origins on the screen.

Are you using named veiws to set your t/c planes?

Kenny

[Allan Brown]

An early Ctour8.dll contour Apps directory patch did not support rotary sub. You could try deleting Ctour8.dll if it exists or download an updated one from the V8.0 patches section.

[JoeyW]

Actually, I noticed that when the Ctour8.dll patch runs, that when MC crashes. I'll try downloading the new one.

Kenneth, My T&C planes are both the same. I am using named veiws for my T&C planes They all have the same origin, so i don't think thats the problem. I'll let you guys know how the new Ctour8.dll works.

 

[Allan Brown]

Getting the part to rotate instead of the tool in the backplot for a horizontal applicaiton is not as intuitive as a vertical application, but goes as follows:

Using toolplanes, enable the Rotary Axis button under Tool parameters. Select Rotary axis positioning with Rotate about Z Axis (i.e. the universal Mastercam Z-Axis). During the backplot Simulate Rotary Axis using Y or Z as the Axis of Rotation.

[RAJ]

i have been reading this subject and would be grateful if somebody would send me an example .

thanks in advance

[email protected]

[nickz]

Yes, I agree with RAJ, I have been looking around for a tombstone style example but have not found one yet. Any help or advice would be helpful. (V8, level 1, 2D or 3D wireframe, no solids)

[This message has been edited by nickz (edited 02-13-2001).]

[d0gFartz]

This things become a real saga......somebody

oughta put all this in a book...............

"As The Pallet Turns"

[Guest CNC Apps Guy 1]

ROFL!!!!!

"As the Pallet Turns"

Yes, In-House should make this book.

James Meyette

[JoeyW]

I didn't mean to drag this topic on for so long.

I downloaded the current Ctour8.dll patch and then it worked just fine. Thanks to everyone for you input. I've created a lot of 4-axis positional programs for our horizontal machine with no problem, but was never able to get the table to rotate in backplot lke everyone said it could. Having the tombstone rotate rather than the tool rotating doesn't help much in terms of verifying if the program is correct or not, but it looks a lot cooler for demos. Thanks again.

Keep those tombstones-a-turning!