RE: [CAD_CAM_EDM_DRO] Re: 2.5 axis vs. 3 axis

Hello Yethdear0

I think I can clear the 2.5d V 3d question with
respect to Dolphin CAD CAM, I am one of the Partners
in Dolphin.

If the Dome exercise is your definition of 3D
then you can say that Dolphin is 3D, your operation
as described can be done very quickly in Dolphin and
the tool used can be a Ball Nose or a Flat End mill.

I attach a Dolphin CAD drawing, CAM file and also
a Fanuc 6M XYZ Part Program showing it. Anyone with
a Dolphin evaluation system can view the Part Program
and anyone with NC verification software can view
the XYZ tool path. The Dome is 80 mm diameter and the
tool used is a 10mm diameter Ball nose. I did not
machine the full dome but only 4 passes, rotating by
one degree for each pass. The surface finish is
controlled by a Dolphin parameter called Arc Tolerance
which is the Cusp Height of the Arc Chord created when
the move is vectored. I only produced 4 tool passes
to reduce the size of the data files being passed
around, if anybody wants the full program then they
can contact me off list.

Well that I believe answers the DOME question.

Now I would like to address the 3D question.

As far as I am concerned for a system to be
able to call itself a true 3D system then it should
be able to machine a complex set of surfaces all
blended and filleted to each other and rising and
falling away in all directions.

CLASSIC EXAMPLES OF THIS IS ARE CAR DASHBOARD,
TELEPHONE HANDSET, COMPUTER MOUSE OR JELLY MOULD.

The various 3d systems available offer different
features such as highy efficient machining strategies,
surface editing etc etc. But the basic test of a 3D
package is the ability to machine parts like those above.

Dolphin CAD CAM cannot do this, and as such we
at Dolphin do not promote it as a full 3d CAD/CAM
product. What Dolphin can do in this arena is :-

Domes
Swept surface
Ruled surface
Rotated surface (male/female)
Patch Surface
Pockets (reguler and irregular) with Angled sides
Pockets where the base contour differs from the top
contour.
Concave/Convex Elliptical Lens shape
Slot, repeated in X or Y or C axes.

There is a lot more, but that is what evaluation is
all about.

Finally as to Windows/DOS :-

Personally I do not find DOS to be limiting, but that
is only my opinion and I have to admit that I get
criticised for driving old Volvos and listening to Steely Dan.

The only Dolphin module currently in DOS is the Turning
module and this is expected to be replaced by JAN/02.

If any further information is required on the above feel
free to contact me off list.

Regards
michael milligan

-----Original Message-----
From: yethdear0 [mailto:yethdear@...]
Sent: 05 December 2001 15:07
To: CAD_CAM_EDM_DRO@yahoogroups.com
Subject: [CAD_CAM_EDM_DRO] Re: 2.5 axis vs. 3 axis

--- In CAD_CAM_EDM_DRO@y..., "Rob" <robv@s...> wrote:
> What's the difference?

Eric & others interested;

I sent this reply once and it didn't post right, excuse my ignorance,
I'm still getting use to this awkward Yahoo BBS.

As for your equipment Eric, If I remember right, your Sherline is a
bench top milling machine using stepper motors? If your machine is
say younger than 10 years old then I would almost bet money that it
could perform a full and true 3D contour.

The Ah-ha control software I am not familiar with. I have seen their
products and been to their web page. I could not tell you for sure if
the software and control would produce a 3D contour or not.

I have not heard of Dolphin software until a few days ago. I take it
that it is an extremely affordable software and it is still DOS
based. (Wow, how limiting!). I read somebody's posting that it was
also cheaper than Bobcad. I would be under the impression that "No",
Dolphin software probably does not have the capability of creating 3D
mesh surfaces and producing contouring toolpaths over those surfaces.
Most low end (cheaper) CAM/CNC software does not have this
capability. Why? Because of the math involved. If you think about it,
for every single move that the CAM software out puts in a 3D type
program, the software has to re-calculate a new contact point that
occurs between the tool and the surface. The results are huge G code
(machining) programs. I have created (with top of the line CAM
software) mold programs that were over 12mb in size and took hours to
run on the CNC.

Try this;
In your Dolphin software, can you construct a 3D dome (hemisphere)?
Will Dolphin then allow you to make a tool path straight across that
dome in the X axis, right across the center of the dome? At the same
time this tool path is made, the CAM software should also produce Z
movements that lift your tool up over the dome and then back down the
other side all the while keeping your tool tangent to the dome
surface. Now, can you rotate that same toolpath ½ degree and repeat
the path and do so for 180 degrees until you have completely machined
the dome surface?

The output from your will be a huge amount of XY and Z points, there
will be no arcs at all. Every single movement and program line should
have an X, Y and Z coordinate value in it. Only circular motion that
is made parallel to any of the 3 main planes (XY, XZ or YZ) can be
output as arcs, as soon as you rotate your motion that first ½
degree, you are no longer running parallel to any of these planes.
This forces the software and computer to output a bunch of straight
line moves (point to point) that will follow the dome. These straight
lines moves will only be as long as the resolution of your software.
Some moves may only be .001 inches or less in length.

If you cannot construct this geometry in Dolphin or if it does not
allow you to produce this type of tool path, then your Dolphin
software is only 2 or 2-1/2 axis.

As for your machine and its control, if you would like to see if it
can do full and true 3D contouring then e-mail at
yethdear@... and I will send you a program to run on your
Sherline mill that will cut this dome shape. This is a simple program
to use to verify what your machine capabilities are. The worst that
will happen is your machine will not simultaneously move all 3 axis
at the same time when it reads a line of data that includes an X, Y
and Z values all on the same line. It will move the X and Y first
then the Z axis last and separately. The result will be a big gouge
in your part. For this reason, you should use a piece of machining
wax, balsa foam, or even a piece of wood so that there is no damage
to your machine or cutting tool if the machine gouges the part.

Here's a freebie tip:

Use "Bondo" auto body filler to make blocks of machineable material
to practice with. The Bondo is nonabrasive and does not dull tools.
It is also cheap and soft enough that if you crash into it, it will
not damage your tool or machine. And if you make a programming
mistake and gouge your block, just add more Bondo and re-cut it. Wal-
mart carries this in the automotive department. Just mix it
separately in one container and then pour it into another container
for molding. This gets rid of air bubbles and ensures mixing. Do be
aware of the fumes and the dust when you machine it.



Addresses:
FAQ: http://www.ktmarketing.com/faq.html
FILES: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO/files/

Post messages: CAD_CAM_EDM_DRO@yahoogroups.com
Subscribe: CAD_CAM_EDM_DRO-subscribe@yahoogroups.com
Unsubscribe: CAD_CAM_EDM_DRO-unsubscribe@yahoogroups.com
List owner: CAD_CAM_EDM_DRO-owner@yahoogroups.com, wanliker@...
Moderator: jmelson@... timg@... [Moderator]
URL to this page: http://groups.yahoo.com/group/CAD_CAM_EDM_DRO
bill,
List Manager



Your use of Yahoo! Groups is subject to http://docs.yahoo.com/info/terms/






[Non-text portions of this message have been removed]