5th axis B rotation not where I want

[Guess_who]

I'm pretty sure this has been discussed before, but I couldn't find the topic. Is there a way to put the B axis exactly where I wand when the A axis is perpendicular to the spindle. For example, if I program a A0 B0 operation, it goes to A0B0, but if I have a previous OP that was at A20 B20, then I do my A0 B0 operation, the code will spit out A0 B20. 

Here is a test program I just made. The 3rd operation is a copy of the 1st op. Notice they are at entirely different B rotations. 

N1 T80050150 M6
(FTN 80050150 - .500 CRIT FIN )
( TEST DRILL ONE )
S4500 M3
G00 G54 G90 A-3. C-3. 
B0. A0.  <---------------- FIRST OP
X-4.4822 Y2.3411
G43 H#999 D#999 Z8. M8
G83 G98 Z-.25 R.1 Q.1 F10.
G80
( TEST CUT 2 )
G65 P9998 E1 B25. A20.  <---------------- SECOND OP
X6.5547 Y6.4304
Z.1
G1 Z-.5
G41 X6.5536 Y6.3804
Y6.3794
G3 X6.5675 Y6.3448 I.05
G1 X10.8678 Y1.8593
G3 X10.9029 Y1.844 I.0361 J.0346
G1 G40 X10.9529 Y1.8429
Z-.4
G0 Z8.
( TEST DRILL ONE )
G65 P9998 E1 B25. A0.  <---------------- THIRD OP
X-3.0729 Y4.0161
G83 G98 Z-.25 R.1 Q.1 F10.
G80
M98 P8888
M30
%

 

[Guest]

Looking at the fact the Op1 doesn't have a G65 line call and OP3 does...

I am assuming this runs through a different section of the post.....

Something is not updating properly...

Try a force tool change on OP3 see if it posts correct positioning then.....if it does, you'll have to look the the other post block to track the variable that's not being updated

 

[mkd]

maybe unrelated to the specific problem, but do you have force tool change on op3?

dang it JP!!!

[Guess_who]

We'll we use a rotation macro here, but when the Part is at A0 B0, it doesn't spit out the macro. This phenomenon happens with all 5 axis posts that I've used.  And doing a force tool change will then reset it and spit out a A0 B0, but what if I want to do A0 B45? And because we are always putting in parts that are too big for our machines we find ourselves running out of Y- travel and needing to force the B to cut in the Y+

So actually that might be a better example. Let say you needed to cut the part at A0 B180. How would you do that without hand editing anything?

[Guest]

Clearly then something is not updating properly then...

I find many times people turn off this post block because they don't like the output at the end

protretinc

This can cause an updating issue.....instead of killing the block....just suppress the output but still update the variables..

I'm shooting in the dark though, as I have no clue what's been done in the posts.

Edited October 16, 2017 by Guest

[crazy^millman]

Well without a bunch of information and some things to work with I think you are asking way to much for someone to help you sort this out. I program things like you are saying all the time and I would have to suspect a post issue 1st and foremost if how you are going about it with your planes and WCS are all set correct. Without seeing all of that and having a lot of other things needed to see more information not much any can offer for help. I hope I am wrong, but to many pieces of the equation missing to get the best answer.

[Guess_who]

The post is a purchased post from an authorized reseller. But to be honest, I don't currently have the generic 5th axis post, but I believe that, that on always did the same thing. 

Actually, I'm not even sure if they supply generic 5 axis posts anymore. I think they may have stopped that.  I wonder if it could be because our 5th axis post is built to have the A0 perpendicular to the spindle. 

[Guest]

Well, if it's a purchased post...

z2g with corrected code and let them handle it....that's what you paid for

[Guess_who]

It was purchased maybe 10 years ago, But I'll ask Jeff to take a look at it. We actually asked a bunch of years back and there was no fix, which is why I figured I'd bring it up again. But it sounds like none of you have an issue with this. 

Thanks for the comments. 

[Guess_who]

So I just re-installed the generic 5th axis post (5 - AXIS TABLE - HEAD VERTICAL)  and it indeed does the same thing. I rotated my plane about -Z- 45 degrees from my top view and posted the path. Yet it posted out C0 B0, and not C45 B0. 

 

:0001(T)
(DATE=DD-MM-YY - 16-10-17 TIME=HH:MM - 11:09)
(MCX FILE - T)
(NC FILE - C:\USERS\RAY1628\DOCUMENTS\MY MCAM2017\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
(T7|13 CENTER DRILL |H7)
N100 G20
N102 G0 G17 G40 G80 G90 G94 G98
N104 G0 G28 G91 Z0.
N106 G0 G28 X0. Y0.
(13 CENTER DRILL |TOOL - 7|DIA. OFF. - 7|LEN. - 7|TOOL DIA. - .25)
N108 M8
N110 T7 M6
N112 G0 G54 G90 X1.8434 Y1.5539 C0. B0. S1000 M3
N114 G43 H7 Z2.
N116 G81 G98 Z-.5 R.1 F5.
N118 G80
N120 M9
N122 M5
N124 G0 G28 G91 Z0.
N126 G0 G28 X0. Y0.
N128 G28
N130 M30

 

[crazy^millman]

27 minutes ago, Ray D said:

So I just re-installed the generic 5th axis post (5 - AXIS TABLE - HEAD VERTICAL)  and it indeed does the same thing. I rotated my plane about -Z- 45 degrees from my top view and posted the path. Yet it posted out C0 B0, and not C45 B0. 

 

:0001(T)
(DATE=DD-MM-YY - 16-10-17 TIME=HH:MM - 11:09)
(MCX FILE - T)
(NC FILE - C:\USERS\RAY1628\DOCUMENTS\MY MCAM2017\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
(T7|13 CENTER DRILL |H7)
N100 G20
N102 G0 G17 G40 G80 G90 G94 G98
N104 G0 G28 G91 Z0.
N106 G0 G28 X0. Y0.
(13 CENTER DRILL |TOOL - 7|DIA. OFF. - 7|LEN. - 7|TOOL DIA. - .25)
N108 M8
N110 T7 M6
N112 G0 G54 G90 X1.8434 Y1.5539 C0. B0. S1000 M3
N114 G43 H7 Z2.
N116 G81 G98 Z-.5 R.1 F5.
N118 G80
N120 M9
N122 M5
N124 G0 G28 G91 Z0.
N126 G0 G28 X0. Y0.
N128 G28
N130 M30

 

That tells me a plane issue might exist. Getting desired output and correct output are 2 different things. Would the output create a good part or a bad part? Not what is the limits of the machine travel. Need to remember Mastercam is not kinematic aware and that includes limits. That is where the programmer needs to create planes and process in their programming to take that into account. I have programmed many different jobs where I use Curve 5 Axis to control move motion and not the left post do work that is doesn't know not to do. You control the process and you make the method you go about it bend to your will not the other way around. If you want the CAM to respect the Kinematics then you need to look at a different CAM since Mastercam is not there yet. There are many things you can do to work within the limits of the Kinematics, but many of them fall back on the programmer to work out and solve with my experience with Mastercam.

Like I have said we need more pieces of the equation and you have only give enough to make me think you need to back up and approach this a totally different way than what you are currently doing to go about this.

How what I solve this problem you might be asking yourself. I would back plot the toolpath and save the retract move from one operation. I would then save the approach move from another. (Thanks Gcode) I would then draw my motion how I wanted the machine to go from one place to the other. I would then use Curve 5 axis to drive that create line or arc. I would then use the approach and retracts to be my tool Axis vectors. I share this example done for a Head-Head to see if it give you an idea what I mean about controlling things.

Example #1

Example #2

If I am wrong and Mastercam can take all of what your asking into account the cool thing is someone will be glad to come in and show me I am wrong. I welcome that anytime since I am self taught and just do my best to get the job done.

[Guess_who]

Thank you for the explanation and examples. Very cool examples by the way. 

And I'm sorry I'm not doing a good job of explaining this.  But put simply, looking at the machine pictured below, what if you simply want to drill a hole with the A0 (as shown in picture) and the C180.

I am finding there is no way to do this without some kind of hand editing the code because MasterCam will Always post A0 C0.

 

[crazy^millman]

You are using one plane with your C0 work and then another plane rotated for your B180 work? A little trick is to sometimes turn your B180 .001 degree and it is enough to trick Mastercam into posting the B rotations is may sometimes miss due the IJK being the same even through they really are not the same. What version of Mastercam?

Edited October 16, 2017 by C^Millman
Question

[Guess_who]

8 minutes ago, C^Millman said:

You are using one plane with your C0 work and then another plane rotated for your B180 work? A little trick is to sometimes turn your B180 .001 degree and it is enough to trick Mastercam into posting the B rotations is may sometimes miss due the IJK being the same even through they really are not the same.

Yes, we create a A0 C180 plane. I'll give your trick a shot. 

Thanks, Millman.  

[huskermcdoogle]

Ray D,

From what I have seen the generic posts don't support the final rotation vector (about the toolplane z), especially when you are at a singularity like A0 C0.  This to me is very annoying, but we live with it.  As Ron has stated, you can cause the math to force it by tipping the plane ever so slightly, and the kinematic setup of the post will make it output very close to what you are looking for, but it won't be exact.  From my limited understanding of the problem, you could write a post which would do what you are looking for, however, it would no longer be "kinematically flexible" such as the generic post is without a bunch of extra logic which would take many man hours to debug and test. 

I have been thinking about this for other similar purposes (top map implementation) and might take a stab at it one day just to gain some knowledge in this arena.

[crazy^millman]

Yes the problem really boils down to a broken method and process in Mastercam is fall back on the programmer ot take a broken process and try to get their job done when makes tons of extra work we shouldn't have to do, but it is the tool we use so we adjust to use it the way we have to.

[huskermcdoogle]

Yeah, more kinematic awareness needs to be put into the base software, this would make the post development side of things to handle issues such as this much much easier.  But at the end of the day, I think there are far too many "preferences" out there and lack of standard conventions to call any one way the right way.  But thinking about it, some of these "conventions" could be worked out if they did a focus group meeting like they did for MT.