5-Axis Hole - Backplots right, Post's wrong

[Reko]

Hi,

 

I am new to the 5-axis toolpaths, so I thought I'd play a bit. I made a block with some simple holes. 4 holes around at 90 degree angles, and two top holes at 10 degrees and 45 degrees at 90 degree opposite angles.

 

When I backplot them, everything looks fine.

 

When I post to check the code, the 4 holes on the outside post correct, but the two top holes post at A-14.1602 C-95.0191 and A-65.5302 C65.5302.

 

Thanks.

[crazy^millman]

1st question is do you have a proven post for that machine? Are you going from the pivot point of the machine or from somewhere else? Do you have the correct axis line defining the center of the hole at the correct angle? Tons of questions before someone could give the best answer.

 

HTH

[Reko]

I have a post, but, admittedly, it isn't complete.

 

I wasn't aware a "pivot" point had to be set and that would affect the angle.

 

I guess I assumed the angle output would be correct no matter what.

 

Also, I did not use a line to define the hole, but a point. then, I set the plane to 3-points using the top hole.

[Watcher]

1st question is do you have a proven post for that machine? Are you going from the pivot point of the machine or from somewhere else? Do you have the correct axis line defining the center of the hole at the correct angle? Tons of questions before someone could give the best answer.

 

HTH

 

The man is back! :guitar: :guitar: :guitar:

[Reko]

I should clarify... I have a post being put together right now from Inhouse Solutions through my distributor.

 

I am just trying to get a head start on understanding the post and how to go about programming.

 

I just received the initial copy of the post, and they did specify that the TCP and TWP were not set up yet due to lack of information on how the tools were to be set up.

 

This is a work in progress, so any information I can get from you guys will help me explain myself better to the post developer.

 

Thank you.

[crazy^millman]

Well there are different methods to describe how a machine works with a tool and a tool works inside the machine. Older machines required we define a pivot distance from the center of rotation of the head if doing head head work, if doing head, machine defined differefent. Thing was everything changes when the tool changes. That happens every time you change a job setup a job or just run a job. This created a lot of extra work for the programmer and the operator. The change in controls allowed you to use a fixed length for posting and then the machine was adjust the tool based off of difference. Now without looking at your file I am not sure where your X,Y,Z zero is. This should again depending on your machine match what you are programming to. Now when you post out you should see the exact angle and go from there if using say G68 work offset shift. It could change if you go off the center of the part. The rotation from center to where your feature comes into place from posting could then change the code to make a good part via how the post is setup. You are following the correct path, just keep working with your dealer and all will work itself out.

 

HTH

 

Daniel, not 100% but better than last week this time.

[Chris Rizzo]

Get a mach sim simulator built along with the post. That will help you immensely too. Every 5 axis move has two choices. Backplot doesn't really show you witch solution.

[Reko]

Thanks 5axisGuy, I have been in contact, so I'm sure we'll get this thing figured out... just not sure why the angles would be wrong... seems like no matter where the pivot point is... the angles of the axis' would have to be correct.

 

@ Rizzo... the owner approved the machsim simulator... so that is also coming soon... looking forward to that too! I know it's not Vericut, but even so, pretty cool stuff as it will help visualize and avoid some mistakes.

[TheePres]

Without looking at file, as we do not have X6 here. Your selection of plane using 3 points might be the culprit for error in vectors.. are these points taken of a true circle normal to hole or of the face of part ..which would make that a spline you are selecting.

[cadman2112]

"TYPICALLY" the first thing to check

 

If it backplots correctly and the angles are wrong, it is almost always a plane that is in error.

 

Double check the path in question and check the orientation of the plane, you'll 'likely" find it's rotated in the wrong direction

 

If it ends up your planes are correct and output is still wrong, you might want to have your reseller look into your post.

[Reko]

Yes, I drew the circles, then tipped them on the angles I wanted so that I could see the output. I even double-checked them, so they are definitely on the correct angles. They are definitely arcs and not splines, as well.

 

Either I am not going about this in the right way, or the post is not correct yet, but like I said, it seems the angles would come out correct no matter what.

 

I was hoping someone would take a look, but no big deal, I'm still a few months away from using the nutating head, and my distributor is looking into it for me.

 

I'll be sure to post the solution for future reference.

 

Thanks.

[gcode]

One thing to keep in mind when using circles to define tool planes.

Every circle has 2 solutions..

Z+ coming towards you

Z- going away from you

Dynamic Planes is a much quicker, safer and more accurate way to define tool planes

[crazy^millman]

Here is what I got for code when changed to a generic machine. You have put Z0 on top of the part. Again question is that where you will set Z zero when programming your parts?

 

%
:0002(TEST_INGERSOLL_POST2)
(DATE=DD-MM-YY - 05-03-13 TIME=HH:MM - 11:34)
(MCX FILE - C:\USERS\RONNINE\DOCUMENTS\MY MCAMX6\MCX\TEST_INGERSOLL_POST.MCX-6)
(NC FILE - C:\USERS\RONNINE\DOCUMENTS\MY MCAMX6\MILL\NC\TEST_INGERSOLL_POST2.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
(T2| 1 INCH DRILL |H2)
N100 G20
N102 G0 G17 G40 G80 G90 G94 G98
N104 G0 G28 G91 Z0.
N106 G0 G28 X0. Y0.
( 1 INCH DRILL |TOOL - 2|DIA. OFF. - 0|LEN. - 2|TOOL DIA. - 1.)
(1" DRILL 3" DEEP - TOP 10 DEGREE ANGLED HOLE)
N108 T2 M6
N110 G0 G54 G90 X.5 Y5.5 C-90. B-10. S1500 M3
N112 G43 H2 Z2.
N114 G83 G98 Z-3. R1. Q0. F6.
N116 G80
N118 M5
N120 G0 G28 G91 Z0.
N122 G28 C0. B0.
N124 M01
N126 G0 G17 G40 G80 G90 G94 G98
N128 G0 G28 G91 Z0.
( 1 INCH DRILL |TOOL - 2|DIA. OFF. - 0|LEN. - 2|TOOL DIA. - 1.)
(1" DRILL 3" DEEP - TOP 45 DEGREE ANGLED HOLE)
N130 T2 M6
N132 G0 G54 G90 X.5 Y4.5 C90. B-45. S1500 M3
N134 G43 H2 Z2.
N136 G83 G98 Z-3. R1. Q0. F6.
N138 G80
N140 M5
N142 G0 G28 G91 Z0.
N144 G0 G28 X0. Y0.
N146 G28 C0. B0.
N148 M30
%

[EX-wccprogrammer]

One thing to keep in mind when using circles to define tool planes.

Every circle has 2 solutions..

Z+ coming towards you

Z- going away from you

Dynamic Planes is a much quicker, safer and more accurate way to define tool planes

 

It is my opinion that there are many more than just 2 possible. A plane can be rotated around the Z axis. This would be indiscernible using a circle for reference, but would create havoc on a post.

[gcode]

It is my opinion that there are many more than just 2 possible. A plane can be rotated around the Z axis. This would be indiscernible using a circle for reference, but would create havoc on a post.

 

this is true, but as a rule Mastercam can assign 2 different views to a circle.

This used to give me fits in V9 days.

I'd create curves from a dozens holes in a solid and use them to define planes for 5X drilling.

Most of the time they'd be right, but sometimes the Z would be out 180°.

Fortunately, the post would ususlly give me an out of range error when this happened.. but not always

[Reko]

Here is what I got for code when changed to a generic machine. You have put Z0 on top of the part. Again question is that where you will set Z zero when programming your parts?

 

That is what I was after. Thank you.

 

I don't know why I didn't think to try a generic post. I tried posting with the Haas 5-axis post and I got the same output as you for the angles, which is what I expected they should be.

 

So, it is definitely the the fact that the post they sent isn't quite ready yet... which is exactly what they told me.

 

Okay... next question... what is your preference for the way you set your tools? Would you set them off the top of the part?

 

Thanks.

[Reko]

One thing to keep in mind when using circles to define tool planes.

Every circle has 2 solutions..

Z+ coming toward you

Z- going away from you

Dynamic Planes is a much quicker, safer and more accurate way to define tool planes

 

Thanks for that tip.

 

I played with the "normal" by flipping it back and forth and it seems the correct position is up, pointing toward the tool coming in.

 

Question... what is your preference for programming 5-axis holes Entity Type... "points," or "points and lines"?

 

Then, for Tool Axis Control, do you like Plane, Surface or parallel to line?

 

It seems like I have to construct something no matter what, so what do you prefer?

[TheePres]

My preference is to use Verisurf hole axis chook and use points and lines.

[crazy^millman]

Tool setting is going ot come down to what the machine supports and gives you for the best use of the control. I assume it is a head machine and not a trunnion, but cannot be sure. If head then set your tools from Z0 on top of the stock if you have always done it that way. Set Z from the bottom of the stock if you have always done it that way. Set them from the Datums if you have always done it that way. Really comes down to what you are using to doing. Now if the control handles the tool lengths then you are good, if not then you will have to get a pivot length for each tool and make sure you post that length according to how the post is set up. IF a trunnion machine then it will be a standard length more than likely and then you will need to have the pivot distance to use in the post to correct differences from where Zero is to where it will move based off of that difference. Your dealer should be able to help you along once you get ot this point.

 

HTH