C-AXIS CROSS DRILLING

[haroldm912]

Hey guys, i am learning to program on our Haas Lathe with live tooling. When drilling a set of holes, as shown in the screen capture, my drill is not coming in on a perpendicuar path to the holes. The drill is tilted at an angle and im not sure exactly why?Basically the drill is not drilling straight. Any suggestions would be most appriciated. i know that cross drill is used for holes that are above or below the center line so it cant be that im using the wrong toolpath.

thanks again!

[crazy^millman]

Well seeing how those holes would require a Y-Axis capable machine and not a C-axis yes I could see where it would not do what you expect since it is not possible to machine those features on a C-axis machine. They would need to be machined using a Mill-Toolpath and make sure the correct place is used for the view you want to machine it in.

 

HTH

[haroldm912]

HI, thanks for the input. however im confused. im following tutorial #8 in the book and it says to choose those options. The cross drill should take that. Is it because my post cannot handle that? Sorry if im not getting it

[haroldm912]

***EDIT*** i can successfully mill those holes, but the tutorial book says to drill them using cross drilling, im just wondering if im not choosing the right options.

[crazy^millman]

Cross drill is an options, but I would think you would be limited to hole on the plane you started with and not around the part like you have chosen. Those types of holes need to be off center and that is where the Y axis capabilities or mill toolpath would be the better choice a toolpath IMHO. I have not idea what workbook you are talking about. I recommend you email them and ask them to provide you a sample file to help you get a better understanding of what is being taught to you.

[haroldm912]

hi millman, it is actually a mastercam7 training book from in house solutions. yeah i agree the milling works just fine, and i would and could choose that, it was just the book said one thing so i was beating myself up trying to figure out why it wouldnt work. thanks again for the help

[crazy^millman]

Okay. Well books are great to learn from, but do not trap yourself to the idea that it has to be by the book. Thing about making parts is the creativity of the person making the program. Let the art of making the part come through in your work. Great you are learning I applaud you for learning. I would not approach a part like what and if they got it to work like that I would love to see the step by step so I could learn how to take something I see as not possible to be possible. My understanding of C-Axis Toolpaths is they must be machinable with C axis capabilities. Those features to me are not and that is where I cannot wrap my brain around what you have told me you were instructed to do.

[#Rekd™]

It looks like your tool plane might be off.

[crazy^millman]

Well I got it to work. I would have thought it would not do it that way, but sure enough even with a C axis Machine it does it. Here is the sample file hopefully the HLE version will open.

 

 

HTH

 

Edited:

 

Download removed email me for file.

Edited November 12, 2013 by Crazy^Millman

[Guest]

Did you use solid geometry for the drilling?

 

Almost always better to create arc and use the wireframe instead. I have seen Tool plane issues related to solid geometry, had to work through QC on that one

[Scott Lundin Shopware Inc.]

If you chain a point it will drill towards center line. You need to chain a circle so it will rotate the spindle to the correct plane and drill what you are looking for. A circle always lays in a flat plane so this is how mastercam knows to rotate to a plane and shift up or down in Y.

[crazy^millman]

I always use Circles for Geometry and then use the pick entity method.