Hi Jasmine, it's a shame that nobody answers you, and I admit I Too cannot help you much!

However, I had a look at the Max Computer site and there is a FAQ and a hotlinel Looking at the personal list, there is at least one English speaking lady (Mrs. Oppl) there. Didn't you get tutorials for that software?

Maybe your problems are something generic, so perhaps you could tell a bit more where your troubles lie. I see there is a demo version available for free; maybe one of the CAD gurus (I'm not, unfortunately) can try a doenload and have a look.

Greetings, Hansrudolf

I have 3ds Max 2012, but mainly use Inventor as my design tool. The general workflow to get from a model to a physical part normally requires an intermediate stage requiring a CAM (computer aided manufacturing) program. The CAM program generates the machine moves (normally G codes as you are discovering) from the geometry produced by your CAD program, or in your case 3ds Max.

Having a quick look at the website for nccad8 it seems that it is available in three versions:

CNC, Standard, and Professional.

The CNC version is purely software to control the milling machine motion and cutting spindle. To use this version you will either have to manually write G codes, or you will have to purchase a separate CAM software package (more of this later).

The Standard version is a CNC controller and a basic CAM package. It will allow you to produce 2D parts from your 3ds models. It works basically with profiles of the part; for example if you were to draw a rectangular plate in 3ds with a few holes in the middle, you should be able to export this model to nccad8 and produce the cutting paths from there. The most common format for this type of CAM work is the dxf file format. 3ds Max allows you to export in this format (click the M symbol upper left and click export, a “select file to export” box will pop up… the various available file formats can be seen via the “save as type” text box at the bottom of the box… use the pull down menu.

The Professional version allows full 3D models to be handled. The most common format used by CAM packages for 3D models is stl format…. Again 3ds Max will allow you to export stl files. I’m not familiar with how nccad handles the process of allowing you to generate the cutting paths.

This process of exporting in an intermediate file format is almost universal with CAM packages, unless you go to very high end versions, and even then I doubt you will find any CAM system that directly handles native 3ds Max formats.

If you have the basic version of nccad8 then you might want to consider a separate CAM package. There are lots to choose from, but most pretty expensive, particularly the full 3D versions. A relatively low cost series of CAM programs are produced by Vectric in the UK. http://www.vectric.com. The two you want to look at are Cut2D (equivalent to nccad8 Standard) and Cut3D (equivalent to nccad8 Pro). The beauty of these is that you can download free demo versions (fully functional except you can only save their sample files). They both come with excellent help files and “getting started” guides. If you work your way thought these (not very complex) you will have a far better idea what is involved generating cutting files from model files, and will hopefully help you understand what nccad8 might be able to do for you.

I hope this is helpful.

Chris

Edited By Chris Courtney on 16/08/2012 20:10:00

What happens if you change the first two I's and J's to negative then the last two to positive ?

Not familiar with a code that doesn't put I's and J's on the same line

;INNER

G0 Y-30

G1 Y30

G3 X-30 Y40 J-10

G1 X30

G3 X40 Y30 I-10

G1 Y-30

G3 X30 Y-40 J10

G1 X-30

G3 X-40 Y-30 I10

G0 X0 Y60

Hi Jasmine

You do not need to go G-code when using nccad, at least not with version 7.5 I am using. Just make a 2D drawing (3D modelling is not possible in nccad) in the CAD part of it, then deside for the technology, i.e. milling: mill dia, depth, speed etc and then start the controller for the milling machine. My version include all three parts; cad, cam and the controller packages, and I can work seamless between them.

For 3D parts to work in nccad a stl file is required. I have litle experience going that way as I am using ViaCad for 3D modeling and Deskproto as the CaM part to end up with a G-code file that is imported into nccad and then going directly to the controller and milling machiine. I am using the Max-computers KOZY Massive A3 **LINK**.

You can import 2D DXF files into the drawing packages but only in DXF version 14. Then give the instructions for the CAM part of it before starting the controller.

Terje

Hi There

A long while since I programmed but:

A couple of things.

I assume the inner is causing the problem? It looks like you are going clockwise around the outside (correct) and clockwise around the inside (incorrect). Also, no obvious G41 either.

You don't have a X start point which should be -40 + at least half the cutter diameter + 1mm or so, probably about -46 assuming a 10mm cutter, but it might have been set up by a previous move.

I think G3 should be G2.

The easy way to remember which way is which is G3 = 3 letters – CCW for counter clock wise and G2 is two letters – CW for clock wise and the program is definitely going clockwise.

I and J on their own are fine john. As the other centre of the radius dimension is correct it is not needed, the program/machine will assume the start point is the radius centre..

I or J 10 or I and J – 10 is just the offset in the direction of the 10 mm radius centre.

The only thing I can't remember is if the + 10 and – 10 and relevant moves should be in incremental. Too long ago since I programmed.

I am assuming that you are cutting the profile outside.

If inside, the cutter must be less than 20mm diameter (10mm radius) or that will stop it working.

Post the complete program as a text file if not too long.

regards David

Edited By David Clark 1 on 02/09/2012 00:44:06

Edited By David Clark 1 on 02/09/2012 00:59:17

Glad you've managed to crack it by yourself, it's a great feeling when you manage to cut your first CNC part on a new machine.

It is useful to be able to program parts manually, but once you get a CAM program working properly and directly importing geometry from your 3dsMax you'll never look back.

Chris