[Xavior]

Hello everyone,

I seem to be having an issue when it comes to interpolating a holes around the 4th axis and my post. I have never done it before, so bare with me as this was my first time.

I have setup the hole profile and wrapped it around the part. Great, everything looked good until it came time to post it.

I posted the process and something strange was happening.

The first hole would goto A20.066
Next line would goto A-20.100

See sample:
N560 G0 G90 G56 X1.312 Y0. A20.463 S3000 M3
N570 G43 H10 Z3.8
N580 Z2.85
N590 G1 Z2.36 F6.
N600 X1.3105 A20.638 F6.
N610 X1.3062 A-20.792
N620 X1.2995 A20.906
N630 X1.2913 A-20.967
N640 X1.2827


Sorry but the numbers above are arbitrary. But for some reason the post is wanting to create this oval shape instead of just interpolating to the bottom depth correctly for a flat bottom with my endmill. I am pretty sure its the post but i could be wrong.. i mean in the mean time what i did was create an interpolation on a flat hole and just manually inputted the 4th axis movements to get it complete but i would like to solve this problem.

Anyone got any ideas?! Could this be related to something other than the post? I am convinced its the post processor that is giving me trouble.

[WallyL7]

Post your file. It sounds like maybe you are needing a 2.5 axis operation and it is posting 3 (or 4) axis code...

[Xavior]

See attached,

Here is my post, its a HAAS VF5 and i have also attached my mc5 file. I am getting errors posting using it, and, it sometimes tells me "more than 1 axis is selected"

Thanks advance!

[WallyL7]

Looks like your WCS and work offsets are in question.

Try this one:

You had a "2" in the work offset for toolpath one which calls for a G56, then the way you had it set up in "planes" prompted the post to add additional offsets instead of just rotating.

[WallyL7]

If you are going to drill this way, the thing you normally need is to have a WCS set up correctly for each position.

Then, when you drill each hole, that hole has the WCS in the initial plane (first hole drilled is the initial), and the tool plane and construction plane in the plane that is actually correct for that hole. This way it uses the initial offset but adds the angle correctly.

The only other way to do this is if you have multi-axis and use a drill 5-axis (with 4-axis enabled) and you would then have all the holes on one toolpath and it would rotate correctly for each one.

[Xavior]

Looks like your WCS and work offsets are in question.

Try this one:

You had a "2" in the work offset for toolpath one which calls for a G56, then the way you had it set up in "planes" prompted the post to add additional offsets instead of just rotating.

Problem now lies when it is posted:

It goes from A190 to A-90

Any ideas?

[WallyL7]

yes - move the toolpaths around.

Put the 4th one first and the current first one third - I think that will make it go ...

0
90
180
270

at least it did for me...lol.

[Xavior]

yes - move the toolpaths around.

Put the 4th one first and the current first one third - I think that will make it go ...

0
90
180
270

at least it did for me...lol.

What function tells mastercam to go from 0 to 90 if the plane always stays bottom? I thought we had to switch the plane around from bottom to left in order to change position of hole in the gcode?

Is my post causing this problem or programming errors?

I am trying to correct the problem for the future when making a new program using the 4th axis. Any tips and hints is appreciated!

[WallyL7]

Do you know how to set up individual WCS's?

You really need to start over on this entire part and add correct (if even redundant) WCS's for EACH hole. They each need to be oriented exactly as they would be on the machine so when you select them the post will be perfect.

By redundant what I mean is you may use the exact same view as one of the default views, but by creating a new view you have something that is more easily recognizable when you are creating the toolpath (since you can name the views you create)

IOW:

Create a view for the second hole and name it Hole #2
then, when you are creating the 2nd toolpath you can reference that view knowing it is in the correct orientation. This part is all 90's which is nice...but what if all the holes are at 10 degrees?


Top view is always the initial starting view (which is bottom in this case)...

This is the code I got with the generic 4axis fanuc post. Your post may be another issue! Try the generic 4axis fanuc to see if it gives you the same code.



%
O0000(TEST)
( T173 | 1 INCH DRILL | H0 )
G20
G0 G17 G40 G49 G80 G90
T173 M6
G0 G90 G56 X0. Y0. A0. S267 M3
G43 H0 Z6.
G98 G81 Z0. R5.1 F4.28
G80
A90.
G98 G81 Z0. R5.1 F4.28
G80
A180.
G98 G81 Z0. R5.1 F4.28
G80
A270.
G98 G81 Z0. R5.1 F4.28
G80
M5
G91 G28 Z0.
G28 X0. Y0. A0.
M30
%

[Xavior]

Do you know how to set up individual WCS's?

You really need to start over on this entire part and add correct (if even redundant) WCS's for EACH hole. They each need to be oriented exactly as they would be on the machine so when you select them the post will be perfect.

By redundant what I mean is you may use the exact same view as one of the default views, but by creating a new view you have something that is more easily recognizable when you are creating the toolpath (since you can name the views you create)

IOW:

Create a view for the second hole and name it Hole #2
then, when you are creating the 2nd toolpath you can reference that view knowing it is in the correct orientation. This part is all 90's which is nice...but what if all the holes are at 10 degrees?


Top view is always the initial starting view (which is bottom in this case)...

This is the code I got with the generic 4axis fanuc post. Your post may be another issue! Try the generic 4axis fanuc to see if it gives you the same code.



%
O0000(TEST)
( T173 | 1 INCH DRILL | H0 )
G20
G0 G17 G40 G49 G80 G90
T173 M6
G0 G90 G56 X0. Y0. A0. S267 M3
G43 H0 Z6.
G98 G81 Z0. R5.1 F4.28
G80
A90.
G98 G81 Z0. R5.1 F4.28
G80
A180.
G98 G81 Z0. R5.1 F4.28
G80
A270.
G98 G81 Z0. R5.1 F4.28
G80
M5
G91 G28 Z0.
G28 X0. Y0. A0.
M30
%

THANKS!!! that makes sense for these basic hole as to why its going A190 then -90.

But for some reason i am having the same problem with something more complicated. Can you have a look for me please?

It looks to be the same concept where i am going wrong but this one has to be started at a specific spot so i am curious what i am doing wrong.

[WallyL7]

I'll try to get to it in a little bit. Someone else may be able to have a peek before me.

Glad that other stuff makes a bit of sense though!:cheers:

[WallyL7]

Is it posting with errors? Not sure what you are having trouble with

[Superman]

THANKS!!! that makes sense for these basic hole as to why its going A190 then -90.

Mark
The sign tell what direction the angle is from A0.
& it all depends on the order of operations, so if you did Front first, you get A-90. but if you did it last,( after doing the other 2 quadrants) it would be A270.

A0 = WCS = your setup
A90 = A-270. = BACK ( new-view rotated around Z by 180°)
A180 = A-180. = BOTTOM ( new-view rotated around Z by 180°)
A270 = A-90. = FRONT

Some posts, & machines are set to travel the shortest distance
if you go A-10. then A10. it ends up being 20° of rotation
you have the same rotation distance if A-10. was put in as A350.

This needs to prove off on your machine, as some do use the minus to force the rotation direction. It also depends on the A-axis settings in the machine definition file.