Getting the results I want out of Mastercam

[KathyM]

I've looked around in the post but I can't seem to find a way to output G12 or G13. G13 is what I really want to use. The Haas I work on understands it but Mastercam won't give it to me. I would like to be able to use it for simple counterbores where the radius of the remaining stock after the hole is drilled is less than the cutter diameter. Pocketing is overkill in this situation. I'm trying to make things easy. Do you think that this _IS_ the post or is there something in Mastercam, itself that I can enable to do this?

I never posted here before. I hope it was the right place to pose this question.

[Gene Newman]

Instead of using pocket, have you tried cirlemill? Can your machines handle G2 and G3 outputs?

[KathyM]

If you mean select 'contour',ye, sure I have. I was just trying to eliminate stopping to figure out the lead-in and lead-out so that the tool comes down in the center of the hole.....

Sometimes that breaks my train of thought.

[Gene Newman]

No, I don't mean contour.

Under toolpaths click next menu, then

circ tlpths, then circle mill. Then pick the dia. you want to cut. On the cut screen set your "start angle" and "entry" both to 90 deg.

make sure you -check- start at center.

This will start tool in center of hole then make one pass to finish dia. and give automatic lead in and lead out. You can use cutter comp or not.

[McRae]

KathyM

 

Create a point at the center of the circle contour. In the operations manager click on the geometry tab under the tool path. Right click inside this and select add chain, chain that point. Now reorder the point above the contour chain, regerate the path and the tool will now start and plunge thru the center of the previously drilled hole.

 

As a new user on the forum, I suggest that you read the FAQ at the top of this list, and secondly, post a file on the CADCAM's FTP sight and we will look at it and assist. The directions to the FTP sight should be in the FAQ or click on the link below the top banner for FTP Instructions.

 

Welcome aboard.

[Keith Graydon]

KathyM,

Greetz, welcome to the forum. Now we have 2 Kathy's! THis is my little fomula for lead-in/lead-out. I have shared this before and i use ita very often. because it WORKS every time.

 

to get tool to plunge on center of a previously drilled hole.

 

Zero out all the fields in leadin/leadout

 

type in the entry field

 

[ Arc Radius =100% ] [(boredia.-tooldia)/4 ]

 

hit enter

press right carat > button to auto fill exit fields.

 

use 180deg entry exit angle

 

again, bore dia - tool dia / 4 = leadin radius

 

 

HTH

-KLG

[Tony]

Thanks Keith!

I had heard there was a

"No need to Backplot over and over till

Your Not gouging" Formula out there...

[KathyM]

Thanks for the tip. I always forget about that next menu. The class I took wasn't very good for real-life situations and since then I'm mostly learning as I go. I'll have to come here and read all the posts. I bet I can learn alot.

[MACHINEMASTERG]

to answer you original question g12or g13 no you wont get that haas code but the way circle mill was described will do what you want welcome to the forum

[Lucky 7]

I would have to agree. I think that the G12 and G13 codes are machine (Haas) specific macros.

[Chris Rizzo]

Yeah, the g12/13 are macros for the Haas...Kathy, it sounds like you might be used to programming at the machine, because the Haas quick code makes it easy to pocket with those g12/13's.

Previous my mastercam experience, I used to do the same.... Welcome to the forum!

[Camdude®]

kathy,

you mentioned that your training wasn't that good. if so please contact your dealer to see if they can rectify the situation.

[kathy]

Kathy,

 

I usually place a point at the center of my circle for a 'pre-drill' and chain the point along with the contour (circle). Than in Lead in / Lead out check 'Use Entry Point'. The reason I don't use circlemill is that my parts have a lot of multi-line/arc cutout contours, so this way I can use a consistent approach!

 

Welcome to the forum.

 

Kathy

[chris m]

Lemme guess Phil; would you be the dealer..?

[KathyM]

I don't know who Phil is and I don't know who the dealer is but my training was on my own. I took a class at Camden County College that was supposed to be "advanced cad-cam". It turned out that it wasn't so advanced unless you never saw a cam program before. I would ask the teacher specific questions pertaining to what I was doing at work and he couldn't always answer me. And then I had to dumb down to keep up with the rest of the class. It was worth taking because I had never used Mastercam before and the company I was working for at the time was about to buy it and I wanted to be one of "the few". I got an A in the class but I still learn something everyday.

[KathyM]

Maybe I should have mentioned that I'm a machinist first and a programmer second. Knowing how to make parts makes the programming easier. I learned programming with a calculator and a pencil with a good eraser.

[chris m]

quote:

---

Maybe I should have mentioned that I'm a machinist first and a programmer second. Knowing how to make parts makes the programming easier. I learned programming with a calculator and a pencil with a good eraser.

---

You are not alone; there are several like you in here (like me, for example). I don't know how much time you've spent on the forum but I'll think you'll find that there is a very good, wide, mixture of talents and experience here.

 

Welcome

C

[MACHINEMASTERG]

kathy i to have taken those classes at camden county and i know what you mean buy dumbing down the rest hold the class back your there for work ..some are there for 3 credits and off to american history... ive found the best training comes from you reseller and this forum... phil /camdude is mentioned above and teaches a great class i think your close to there location ???"hey phil how about a free t shirt for the plug"