Re: [CAD_CAM_EDM_DRO] Please take a look over my shoulder – CAD CA M CNC Bench Mill System

Hi Whelen,

Wow, you have managed to ask a lot of question in one posting :-) OK,
I'll do my best to help.

First CAD/CAM. Think about the sort of work you want to do. You
automatically assumed you need 3D CAD/CAM. Do you? 3D is great for mould
making and 3 dimensional carving but it is not ideal for more
'conventional' work such as engraving or general purpose milling. Quite
a few people have bought expensive 3D packages and found out they are
better off with 2.1/2D. Could a skilled machinist cut the parts you
want, assuming he/she could operate both X and Y handles at the same
time (Or X and A for a rotary axis)? If so, you only need 2.1/2D. With
2.1/2D machining the Z axis does not move with the X and Y. This is like
most manual milling. You set the cut depth then take some cuts, change
the depth then take some other cuts and so on.

With engraving it is often a good idea to use a 'floating head'. The
cutter holder is mounted on some form of slide mounted on the Z axis so
it can freely move up and down with a light spring to push it down. The
cutter projects through a guide nose that touches the work and controls
the cut depth. Any variations in the surface are followed by the guide
nose, keeping a consistent cut depth. You can engrave onto curved
surfaces using this technique. In extreme cases there are guide noses
available that use a ball with a hole drilled in it. The ball is free to
rotate in any direction and the cutter runs through the drilled hole.
This will follow even quite steep angles. You could instead use a fixed
cutter and use 3D CAD to draw the part you are cutting but your drawing
will have to be very accurate. For instance if you are engraving .005
deep, your drawing will have to be accurate to 0.001", not easy
especially if the ring is hand made and not perfectly accurate.

For normal engraving you would probably be better off with a good 2D
'artistic' CAD package and 2.1/2D CAM. A lot of engravers use CorelDraw.
It is relatively cheap and has a huge array of text handling facilities.
Combine that with a good CAM package and you will be able to do pretty
much any engraving job. Corel's big downfall is that it is not great for
precision engineering work. For that you are probably better off with a
more conventional CAD package. DesignCad Express
(http://www.upperspace.com/) is ludicrously cheap at $35 and is actually
quite good. One nice feature of DesignCad is that it comes with it's own
single stroke fonts that engrave really well. Ordinary Windows TrueType
fonts don't engrave well if you are doing small work.

For CAM I would suggest giving SheetCam (www.sheetcam.com) a try. It is
$150 and works very well with CorelDraw or most other 2D CAD packages. I
admit I am slightly biased here, being the author of SheetCam.

Your best bet is to download all the demos you can get hold of and have
a play. Software that suits one person may not suit another. Try to find
something that you find easy to use.

If you have the choice between stl and dxf, I would choose dxf. DXF
files fully describe the whole object. For instance if you draw a circle
a DXF file will specify a circle. STL files just describe the surface as
a mesh of triangles in 3 dimensional space. A circle will be
approximated by a large number of triangles joined together. This makes
things a whole lot simpler for the CAM software but does reduce accuracy.

You don't appear to be too sure how all the software components mesh
together so here is a basic workflow which may clear things up a bit.

1) Draw your part in CAD. This could be a 3D model or a simple 2D
drawing. It helps to keep in mind how you are going to machine the part
as you draw it!

2) Import the drawing into CAM and apply the tool paths. The CAM takes
your drawing and works out where the cutter has to run to machine the
part you have drawn. You have to provide a fair amount of input
specifying how you want the part cut and what cutters to use. Your
machining experience will help a lot here.

3) Once you have created the tool paths the CAM uses a built in program
called a post processor to generate the G-code file. G-code is just a
sequence of movement instructions for your machine. G-code gets it's
name from the instructions, most of which start with the letter G. Some
instructions use the letter M but they are still called g-code.

4) Load the G-code into your machine controller. This can be a dedicated
machine or software running on your computer such as
Mach2(www.artofcnc.ca) or Turbocnc (www.dakeng.com). The machine
controller takes the g-code and converts it into electrical signals to
the motor drives to actually move the machine. It also takes care of
jogging, zeroing coordinates, coolant etc.

On to the mechanical side:

How much torque do you need? This is the most difficult question. It
depends very much on your machine. Think of how much torque you have
needed to apply to the handles when using this machine. Estimate the
maximum you have ever needed to apply while taking a heavy cut. Use this
as the continuous torque rating of your servo drive system. This is a
very conservative estimate but you are better safe than sorry. Once you
have this torque, find out what the continuous rating of your motor is.
The ratio between these two values will give the reduction ration
needed. For instance if you estimate you need 400oz-in to turn the
handle and your motor is 100 oz-in then you need 4:1 reduction. Toothed
belt is ideal because it gives you the option to easily change ratios if
you get it wrong. Your rapid speed will be the motor maximum speed
divided by the reduction ratio times the screw TPI. Say the motor can do
4000RPM and your screw is 10TPI. The rapid speed will be 4000/(4 * 10) =
100IPM - this would be plenty fast enough.


Should you replace the lead screw nuts? Possibly if they are worn. You
want to do everything possible to reduce backlash. Ideally you should
replace the screws with ballscrews as CNC machines are less tolerant to
backlash than manual machines. Theoretically the software can compensate
but in practise it is not an ideal solution. Ballscrews are expensive so
I would suggest running with the current screws for the time being. The
machine will work with them so you can upgrade in the future if you find
the backlash is a problem.

Should you loosen the gibs? NO! Keep them just loose enough to move
freely and use plenty of good quality slideway lubricant (not engine oil).

Should you lap the ways? Would you if you were keeping the machine for
manual use? Lapping should be done with care or you can make things
worse rather than better.

I hope that has helped answer some of your questions,

Les