Rotating a fixture offset on a Thermwood Model 67

[JSP Mold]

Does anyone know if it is possible to rotate a fixture offset when using a Thermwood Model 67 5-axis router?

For example, a fixture offset that is rotated 45 degrees around the "Z" axis, and then rotated 20 degrees around the "X" axis.

If so, can the rotation of the offset be set "on the fly" from within a program?

[Dan Bedore]

are you trying to do a C axis and B axis move then cut with X,Y,Z? if so yes send me a simple file and i will show you how to set it up. if not what are you trying to do?

[crazy^millman]

Well jps why dont you just rotate the Cplane and Tplane to that plane and start Machining from there. I write all my programs from one workoffset the just postion my cplanes and tplane accordinly. If I wans to do multi part then I just use the G52LXX as my program location for each part if using the same tool and go from there. The model 67 does have -135 to 135 on the B axis so sounds like it is within that work area.

 

Crazy Millman

[JSP Mold]

It is kind of hard to explain in writing what I am trying to accomplish, but I will try to do my best to explain it.

 

The molds we build are not like plastic injection molds where a cavity is cut into a moldbase. Our molds are a "shelled" core/cavity type of mold. Our parts are made up of complex "sweeps" and very rarely have any planar surfaces. Anyway.....

 

What I am trying to do is, to core vent the majority of our cavities using our new 5-axis router.

Each cavity can have anywhere between 75-300 core vents that need to be drilled into each cavity.

 

A core vent is virtually a 3/8" diameter hole drilled from the backside of the cavity to within .050" of breaking thru the inside of the cavity. At the bottom of this "back-drilled" hole are a series of (19) 3/32" diameter holes spaced out in a circular array. These 3/32" diameter holes get drilled thru the .050" thick floor of the core vent and into the inside of the cavity. Each one of these core vents has to be perpendicular to the inside surface of the cavity. Which means that every core vent has its own "B" axis and "C" axis rotation values.

 

I have no trouble getting the 3/8" diameter "back-drilled" holes into the part. The trouble lies in getting all the 3/32" diameter holes put in in a timely matter. Machining time isnt the factor here, its the layout and programming of all the 3/32" holes. I would like to layout 200 points, for example, on the inside of the cavity, use those for my drill points when drilling the 3/8" holes, then use sometype of sub-routine to drill the 3/32" holes. But, Mastercam doesnt currently support sub-routines in 5-axis drilling.

 

When speaking with my MC reseller, he mentioned that some 5-axis machines have the ability to let the program position and rotate the head in the correct orientation, and then set a fixture offset so that the "Z" axis is basically running up the shank of the tool. Lucky for us, we are drilling the 3/32" holes in a circular array, so the direction of the "X" and "Y" axis would really matter, just the "Z" axis. From there we could call up a incrementally programmed sub-routine to drill the 3/32" holes. Once completed, change the offset back to its original state. position to the next hole, and continue the cycle on around the rest of the part.

 

I realize this relpy has become a bit long winded, but like I said, its kind of hard to explain in writing. Hopefully I have been detailed enough so that everyone gets an understanding of what im trying to do!!

[crazy^millman]

But yes you can still do what I am saying this way. You can also do a sub program for a 5 axis drill just have to be tricky about it all and you could easliy do an incremtnal shift as well. The thing you have to remember about the Thermwoods is that the sub directory is funky is all. I know it require a little work but let take a gris patter of 10 holes. i would do one sub program as a incremental shift then I would do the other program as my incremtnal depths if doing ti the sub program route. You can do it the in one progrma using the M80L, M81L, and M82L as your absoulte location calls.

 

I know you are shakeing your head but just bear with me here. I have set up my post ot support the 5 axis circle macros. I did this but usign the Misc 2 anf the change the psot to output the way I wanted. It is using a 5 axis drill for the control for the axis rotation for the C axis and the B Axis then it take the input for the Depth, Retract, Feed to the vaules needed to do the Cicrle Macro. Well what I suggets is that you need to get the information for those points realtive to the povit distance for the tool you are going to use. If you create a drill operation to act as your template for the needed information then it is just a point and shoot away from that.

 

Here is what a smaple cose would look like:

 

code:

---

 HAVE TO FINISH THIS TOMMORROW 

---

 

[ 01-13-2004, 08:28 PM: Message edited by: Millman^Crazy ]

[JSP Mold]

Millman,

I understand what you are saying about using the M82L# to call up a label that starts with M80L#.

 

With the way you suggested, would I be able to use the same label to drill the same hole pattern on 5 sides of a cube for example? I would think that I would need seperate labels (one for each side of the cube)to drill the hole pattern on 5 sides of the cube. Wouldn't the XY positioning of the label be different for the top plane of the cube, as opposed to the right plane, which would be YZ position moves?

Each one of my hole patterns is going to have a different "B" and "C" axis rotation. If I have to create a T/C plane at each one of the pattern locations thats fine. Its going to take quite some time to do, but it will get the job done. If possible, I would like to find some way so that I dont have to do that.

[Dan Bedore]

i think you could speed up some of this by using fplot to either set your vectors and or creat your planes. something like Iskander teh

showed in his post, Variable pitch threads ,anybody interested ?!?

I could't tell you how to do it but I bet some one out there can.

mastercam forum

[crazy^millman]

Well Not really if they are all the same you creat everything on one plane. Take the front plane for example. You create everythign you need on that plane and then do a transform with sub program you can then so a incremetnal sub here and that si your data for one of the subs but if you do it right I think you will get data for 2 sub. My post will break all the postion locations into the main and then it will put allthe drilling information into a subprogram using transform and subprograms this way. If you want opt have gemontry on all side of the 5 axis part and it is the same then you can do xform/rotate.

 

Let us say it is all different on each side but they are all the same pattern then you would creat the 5 c-planes you need and then do the start for the frist. You would then need to do the the pattern call for the first sub and then the pecking routine for the second sub. This even works greta fi you have different depth holes then you would have one sub peck as .5 depth realtive to start and then you could have others like .75 deep and so on. I know it seem like alot of work but doing this for one hole and just doing the incremental shift is going to save tons of time on 200 holes. The programming will be eaiser and faster this route then picking all those 200 places.

 

I also believe there is a chook that will put pounts in the center of all holes. If not I think you could easily talk to Mick and he could write a script to do this on a part. Good Luck

 

CraZy Millman

[JSP Mold]

Thanks for your suggestions Millman! I will give them a try and let you know how things turn out.

 

Anyone else have any suggestions on this subject?

[Pierre Côté]

My suggestion here is :

 

Are you able to defined the points positions with a line attached to it as the tool vector direction ?

 

Then use Drill 5ax to perform the holes.

[crazy^millman]

Well that is what I was thinking on the Chook then if the are put on a different lable then you can create a line between them. I do know how involved it would be to take and write a chook ot a script to see the hole create a point at each and then create a point bewteen those 2 points and not to every other point on the part.

 

Crazy Millman