Drilling at a negative angle

[wdg5555]

I'm trying to figure out how to get mastercam to post out a negative angle on my drill toolpaths. I'm running a mill/turn machine.

 

I have some holes I need to drill at 6.5 degrees. I want to drill them at a -6.5 degrees on the machine. I can get mastercam to post out the program correctly for 6.5 degrees, just don't know how to force it to drill at -6.5.

 

Right now I'm posting it out at 6.5 degrees and changing it to a negative and also changing my c,x, and y values so it drills in the correct place...surely there is an easier way?

[K2csq7]

Got a file to share?

Screen shot?

What kind of mill/turn machine?

[wdg5555]

Attached is the file I am working on.

 

I'm running an Okuma Multus B400.

TT.MCX-5

[EX-wccprogrammer]

Some posts have logic that keeps rotations between 0 and 360. If this is the case with your post, you never will see a negative unless you go in and edit the post.

[K2csq7]

What do you have for misc integers for your post/MD/CD.....

Do you have one that says "start solution" or something like that?

 

I switched that Misc integer on my integrex post and it spits out....

 

O0000 (CB12373 TOP)
(CB12373 TOP)
(MASTERCAM - X6)
(DATE = 12/23/2013)
(TIME = 1:34 PM)
(POST = MPPOSTABILITY_MAZAK_I_SERIES.PST)
(T21 - 11/32 JOBBER DRILL - D21=0.0)
G00 G17 G20 G40 G80 G90
G91 G00 G28 X0.
G28 Y0. Z0.
N1
(BA=-6.5, REVERSE X AND Y)
G10.9 X0
M901
M200
T21 M6 (11/32 JOBBER DRILL)
G91 G00 G28 X0.
G17 G90
G54
M108 M212
B-6.5 C90.<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
M107 M210
G68 X0. Y0. Z0. I0. J1. K0. R-6.5
G97 S465 M3
G43 H21 X5.0228 Y.4 Z.6527
G94
G98 G82 Z-2.3473 R-1.2973 F2.
G80
G69
M5
G91 G28 X0. Y0.
G28 Z0.
G49
M30

[crazy^millman]

There is the answer that is a pst control setting using a mi value in most posts. Get on the horn to your PP company and see what they did when they made your post for you. I see it looks like a Mill Post and not a Lathe Post so looks like you need to purchase one.

 

Also on that file I would strongly recommend you look to the multi-axis drill toolpaths and post all of the hole in one operation and be done with it. Will need to have the center line above the hole not below like you currently have it. Also make your points in the center of the holes and all of those holes will be done in a few seconds of programming.

 

HTH

[crazy^millman]

Also I would suggest you contact your dealer about the MT product for that machine. With PP, Simulation and other things all dialed in pretty nice in X7.

 

HTH

[wdg5555]

Thanks for the help. I looked under my misc integers and there wasn't any option for my problem. Looks like I'll have to do some more post editing

Also on that file I would strongly recommend you look to the multi-axis drill toolpaths and post all of the hole in one operation and be done with it. Will need to have the center line above the hole not below like you currently have it. Also make your points in the center of the holes and all of those holes will be done in a few seconds of programming.HTH

Not sure what the multi-axis drillpaths are or where they would be. I'm not sure I can use those though since we do not have the Multi-axis addon for our Mastercam.Also with this part I run into the X axis limit. I have to program half of the holes at 6.5 and the other half at -6.5(I don't have as much travel in X when I'm at Y negative).

Also I would suggest you contact your dealer about the MT product for that machine. With PP, Simulation and other things all dialed in pretty nice in X7.HTH

Not sure what the "MT product" is. I'm assuming its some sort of virtual machine? Haven't done too much with X7. The verify seems to crash alot for me.

[Watcher]

Most Millturn posts have logic to keep the solution on the positive quadrant as most millturns have limitations on "-" side of X axis...

 

Just out of curiosity: Why 6.5 and Cx would not work for you? I'm assuming you current PP is also rotating C so Y is kept at 0 right?

 

Can't you program at B6.5 and rotate C for every hole?

 

I'm afraid you will have to code this by hand for now...

[wdg5555]

Most Millturn posts have logic to keep the solution on the positive quadrant as most millturns have limitations on "-" side of X axis...

 

Just out of curiosity: Why 6.5 and Cx would not work for you? I'm assuming you current PP is also rotating C so Y is kept at 0 right?

 

I'm afraid you will have to code this by hand for now...

 

All the angled holes for this part are not at Y zero. And the holes that are at Y+ I can do at 6.5 degrees. But I run into the x axis limit when I go to Y negative so I have to rotate the turret to -6.5 degrees and stay on the Y+ side.

 

I think I can edit my post easily enough to get it to work for me. Just use a misc integer as suggested above.

[Watcher]

All the angled holes for this part are not at Y zero. And the holes that are at Y+ I can do at 6.5 degrees. But I run into the x axis limit when I go to Y negative so I have to rotate the turret to -6.5 degrees and stay on the Y+ side.

 

I think I can edit my post easily enough to get it to work for me. Just use a misc integer as suggested above.

 

I see your geometry now...

 

I noticed you're using a PP from Dave... are you sure the portion with the logic you need to tweak is not binned?

[crazy^millman]

MT is the Mill Turn product that came out in this version of Mastercam. The file I opened show a MULTUS B300/B400 - W which they have done tons of work on.

 

5 axis drill toolpath where you use points on the center of the circles and then use lines on the center of the hole to control the Vector.

 

Watcher I am pretty certain this is just not being used correctly since almost every PP builder I know puts that switch in their post, Dave's included and he is on Vacation this week so he will have to wait to next week if he wants a post edit.

[wdg5555]

Watcher I am pretty certain this is just not being used correctly since almost every PP builder I know puts that switch in their post, Dave's included and he is on Vacation this week so he will have to wait to next week if he wants a post edit.

 

I won't wait until Dave gets back. I'll do it myself

[crazy^millman]

I won't wait until Dave gets back. I'll do it myself

 

Wow I am very impressed you have a fully unlocked post of his to do that in.

 

Though I have to say if you knew how to edit the post and do that why did you even bother to come into here to ask for help?

[GIZMO 21]

 

 

Wow I am very impressed you have a fully unlocked post of his to do that in.

 

Though I have to say if you knew how to edit the post and do that why did you even bother to come into here to ask for help?

 

Seriously i have alot of respect for you,but sometimes your a pain in the xxxx.and i know i dont have a large post count before you point that out.

[Watcher]

Though I have to say if you knew how to edit the post and do that why did you even bother to come into here to ask for help?

 

Maybe he was asking for advice on Mastercam side?

[crazy^millman]

Gizmo not really sure why I have it, I am just trying help sorry I hate my high post count and they could do away with them. I gave Mastercam help and gave insight into his incomplete file that had limited information. I also made a suggestion about the PP and I am impressed he know how to work out the part of a post.

 

To others if my remarks came across the wrong way I apologize for that. I see people come in for help like this and never come back or pop in only once in a while. I would love to hear how he worked out taken a locked up section of post and trick it to do this. If he has one of Dave's post he charges for that is fully unlocked where he does not have to worry about that then like said i am vey impresed. Simple people are easily impressed and reading this person posses that ability I wold love to have a person who is a lot smarter than me come in here more often so I can learn from then. Again sorry it came across the wrong way.

 

Have Merry Christmas.

[crazy^millman]

Watcher he had one operation with a plane for his indexing was about as Mastercam as you get for such a simple feature. I seen as a PP issue like others so why I was confused again sorry.

 

 

[wdg5555]

Maybe he was asking for advice on Mastercam side?

 

Ya, this was it.

Thanks again for your help.

[K2csq7]

Ron hit the nail on the head..

Though I have to say if you knew how to edit the post and do that why did you even bother to come into here to ask for help?

 

I am with you Ron. If you have the expertise to make an edit like that..... well..... in the time it took to make this thread, he could have been making chips.

 

I smell something fishy...

[blue hootie]

drill at 353.5 degrees,

[wdg5555]

I am with you Ron. If you have the expertise to make an edit like that..... well..... in the time it took to make this thread, he could have been making chips.

 

I smell something fishy...

 

I was already finished with the job when I posted this question. Like I said above I post it out and then change the angle, x, y, and c numbers. And I'm not an expert at Mastercam or at Post editing. Especially post editing. But I like to learn and the best way to learn is by doing. Hopefully I will be able to edit it. I think I have a good plan to change all of the numbers except I'm not sure about how to change it in the drilling canned cycle. Haven't had time to start working on it yet. I've had very very little training on post editing. Its all trial and error.

 

The other reason I like to do my own post edits is I found it to be a pain to send it out. The last time I tried it the post came back worse than it already was. And half of the edits I asked for were not done.

[crazy^millman]

Sorry, but then I know you are not dealing with Dave at Postability of whom we were talking about. The drilling cycles are very easy to change, but this is not a dealing problem issue. This is a matrix math problem. Inverseing the vector math and having the X-Y-Z-A-C come out correctly is IMHO not simple task. The base Matrix in which the code is coming from is one part of the process, but now reversing the logic to know to stay in the upper half of the X when the Angle start to switch if you were going to do it as a 5 Axis toolpath would be quite a chore. Doing in single operations would work and then putting in the logic in the math part of the post when the trigger is used to force the negative angle is doable, but again will be quite a task to make sure you keep the math logic correct while not messing with the output logic. Formatting the variables correctly and controlling the trigger should be pretty straight forward. I have done post edits for years and be cool to see how you work it all out. If I can be of assistance I will be glad to help out.

[Watcher]

Very well put Ron... No matter how motivated you are wdg5555, this is not an obvious mod in the post kernel from my experience...