Re: [CAD_CAM_EDM_DRO] MASTERCAM

Hi Vic:
Sorry it's taken so long to get back to you; I had kid duty all day
today.
I'm having trouble visualizing what you're trying to achieve, so if my
comments are incomprehensible, bear with me.
As I understand it, you are trying to create a partial arc in the Y-Z
plane???
You are then trying to create a toolpath to follow the arc???

If this is actually what you're trying to do, then there are two basic ways
that I know of, to go about it.
Way number (1) involves creating the code as an arc move and then using
plane switching to flip it into the correct plane.
This is done on many controls with a G17 or G18 command. Mastercam will not
help you here so far as I know.
The other way is to create the arc geometry in the correct plane in
Mastercam and then approximate the arc move by using a 3D contour toolpath.
In version 7, there is not yet a dedicated 3D contour command, but you can
get there by setting the contour depth as "incremental", setting the
compensation in computer to "off", the compensation in control to "off", the
tip comp to "center", and making sure that the arc you drew is offset
properly so you end up cutting the shape in the right spot.
YOU WILL GET A TOOLPATH THAT IS COMPOSED OF SHORT LINE SEGMENTS!!!
The moves will all be G01 moves.

To recap in detail:
1) Open Mastercam
2) select "G view -side" This gets you into the Y-Z plane.
3) select "create-arc-circle point dia" then enter your coordinates and
sizes.
4) select "create-line-horizontal" and place a cut line.
5) select "modify-break-intersection" and break the circle at the cutline.
6) dump the part of the arc you don't want and the cutline.
7) select "toolpaths-contour" and select one end of the arc.
8) Right click anywhere in the window that opens, and pick your tool from
the tool list.
9) Set your tool parameters per your preferences.
10) Click on "contour parameters" to get into the next dialog box.
11) Go down the list, filling in the boxes. When you get to "Top of stock"
and "Depth", make sure the radio buttons for "incremental" are both
selected, and the values in the boxes are "0".
12) Compensation in computer and compensation in control should both be set
to "off"
13) Tip comp should be set to "center"
14) Linearization tolerance should be set pretty small; 0.0002" is good.

Now you can run the simulation to see if your toolpath is as expected.
You can edit the parameters as needed to change just about anything in the
toolpath.
When you post it, you will find it is a big file (comparatively speaking)
composed of G01 moves.

The value of doing it this way as opposed to the non Mastercam method, is
that you can get this toolpath to run along any contour that you can draw.
Mastercam doesn't care if it's a wiggly NURBS spline, a bunch of lines and
arcs, or a bezier curve projected onto a surface in 3D.
So it's a really versatile way of picking out cavity corners for example.
I also use it when I have to machine an undercut with a lollipop type
cutter.
I can throw a bunch of flowlines on an undercut surface and bomb a cutter
along the contours.
This is great for the antirock undercuts in bottle moulds.

A great resource I have found for questions like these, is the Mastercam
forum.
You can ask just about anything there and there are some REALLY smart people
on the list.
I don't know the URL offhand, but a search should bring it up pretty
quickly.

Cheers

Marcus

-----Original Message-----
From: Victor Cantu Jr. <victorcantujr@...>
To: CAD_CAM_EDM_DRO@yahoogroups.com <CAD_CAM_EDM_DRO@yahoogroups.com>
Date: Friday, March 30, 2001 9:24 PM
Subject: [CAD_CAM_EDM_DRO] MASTERCAM

>MARCUS,
> well in the weeks to come I have a really tough part, but

just today I am struggling with a simple Y Z circular move. what I want to
do is make an arc using a 3/16 ball end mill. the radius is 1.437 I want to
start this at X 2.375 Y-2. Z-.05. and end it some place over the part ..2
to .3 over I tried to write this out by hand but my machine called me stupid
ha ha . All I got was a calculated radius error. I am running a Fadal 15XT.
DO YOU THINK YOU CAN HELP ME WITH THIS LINE?? I HOPE SO

>
>

VICTOR