Fadal rotary table

[Joels]

Hello, Our old Fadal 4020 has a rotary table in that points verticle. I need to program this using Mastercam. The current programmer uses V basic and alot of math. The problem is i need to cut the part by using the tool on z axis only and have the table turn to machine x,y. Anyone know how to do this?

 

Joel

Mcam X4

[crazy^millman]

Go into the machine def and define the way the 4th axis is set-up and then it should work for you. You may have to use axis sub or even C/T planes to get the rotations you are after.

 

HTH

[Justin Beebe at Folsom Tool]

Joels

 

Is it a 4-axis clamped down vertical or a 5-axis tilted vertical?

[Joels]

Hello. I am back at this problem again. I have a rotary table on the Z axis. The part and table are too big for the machine so right now we bring the tool down to the part at a specified location and as the tool moves in Z axis the table turns. I can get the table to turn but how do i get the tool to stay in one point in X and Y while feeding on Z axis?

[Bryan Johnson]

Assuming the rotary is rotating about the Z axis, select the “Rotary Axis Control” page from your toolpath parameters.

Rotation Type = 3 axis

Rotary axis = Rotate about Z axis

 

This will give you a toolpath motion using X and the Rotary.

The default post should support this without needing to modify the machine def.

[Joels]

Bryan, thank you for the reply. I did selct the 3 axis option and the table does rotate but the I am seeing moves in the output that suggest the tool is moving too. The table has a very small area to move in because of the large part we have in the machine. The part over hangs the table on a 4020 Fadal. I need the tool to position itself in X and Y and stay in that position and only feed in Z axis whole the table turns. the table is on the Z axis. I am not at work now but i can upload the file tonight if that helps.

[taperlength]

That's only going to work if you are machining circles. It will have to move either X or Y to do other contours.

[CJep]

Joel,

You will need to go into your machine definition in the machine group properties and make a setting for the A axis properties

 

Open files in the machine group properties, select edit. In the machine definition manger select VMC A axis and right click to open the properties. In the upper left of the A axis component manager you will see "World Coordinate System", change the axis of rotation for the A axis to "Z", green check your way out to accept the changes and repost.

 

By making the changes through the machine group properties it will only affect the part file not the default machine definition

[Joels]

Cjep, that works good. I checked the box next to that one by mistake. too much of a hurry. now the program is 700 lines long, its like each block moves the table one degree, how do i change that?

[CJep]

I hate to say this but I haven't been able to find a cure for that one.

 

 

Something I do know, it takes 43 muscles to frown, 17 to smile but only 3 for proper trigger squeeze.

[CJep]

When I output the code using a 12.5dia closed arc the move is broke down to every 1.4173deg.

 

I used the trim break utility; break circles and broke the closed arc into quadrants. The code is still output in 1.4063deg increments, however the code I'm getting is broke down in 11.25deg sections.

[K2csq7]

In the Mach. def. double click your rotary axis and then in the bottom left there is a break rotary motion checkbox. I am not sure if this is the cure your looking for, but it sure sounds like it.

[CJep]

Yeh, I tried that earlier, it sounded like a solution but had no effect. I have a feeling this has more to do with how the NCI is breaking down information and sharing it with the post

[K2csq7]

Anyone know what that setting is for?

[CJep]

Set the axis type to signed direction, that will make for some serious weirdness in the code, not certain if this will cause smoke to roll out of every orifice of the control panel. I'm fairly certain the Haas VF control wouldn't see the humor.

 

N120 T2 M06 ( TOOL - 2 1/2 FLAT ENDMILL / TOOL DIA. - .5 )

N130 G0 G90 G54 X6.775 Y0. A0. S2650 M3

N140 G43 H2 Z.125

N150 M08

N160 G1 Z-.5 F50.

N170 X6.5 F25.

N180 A-358.6364

N190 A--357.2727

N200 A---355.9091

N210 A----354.5455

N220 A-----353.1818

N230 A------351.8182

N240 A-------350.4545

N250 A--------349.0909

N260 A---------347.7273

[Joels]

I turned on "rotary axis positioning" and the code was about 7 lines long when it was 700 lines long. works good now.