Kosy nccad8 HELP!

Hi guys

I have purchased a Proxxon FF500 cnc which came with Kosy Nccad8 software.

Everything is setup and installed I just can't figure out how to use nccad8!

Have emailed Kosy a number of times for a simple tutorial and keep getting no help!

I spent £4500.00 on a machine which I can't use.......please help I'm going crazy trying to figure it out.

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 Googled nccad8 & on this page :

http://www.max-computer.de/x5e/download_nccad8_help.html

is a downloadable html based manual ? I have had a quick look at this - it downloaded Ok and runs, but I have not checjked out how much depth it goes into. Might be worth a look ?

Regards,

Nigel B.

Thanks for replying boys,

I have read through the manual a number of times also viewed the help videos via the in app help menu.

I am that desperate I am now learning G- Code to get things started.

However; I have used 3ds max for a while and would say I am pretty good with it.

Is there a way of converting a 3d model to G-Code so I could just copy / past the code into Nccad?

At 4.5K you must have bought this new as Axminster offer it at just under this price. Your supplier should be able to help in some way. I must say it is a dinky little machine compared to the Sieg KX3 for similar money, which uses the more well known Mach3 for control (and a number of built-in wizards for 'standard' machining tasks), and Cut-2D (2.5D which is all you need) for converting CAD produced DXF file into G-Code/CNC tool paths for processing by Mach3.

The user manual is available on the Axminster site and it says:

"After the program was successfully installed, it can be started just as you are used to from other applications on your computer. Simply select the "Start" button on the screen with your cursor and select the desired file in the program title bar. It's even easier if you simply click the program icon.

We deliberately refrained from using a printed form of the manual and, as already mentioned above, have consolidated the necessary contents in a help function within the program itself. A much more practical and neater possibility than having to handle a mountain of paper: The structure of the topics has been optimised for an intuitive and self-explanatory entry; important things are recognised first and navigation afterwards is effortless: In the normal view, click on Help in the menu line at the top right to start the "Help Function". A submenu appears: click here on Help topics and then the Help window will appear."

So it looks like you are going to have to sit down at your PC and get learning the hard way.

Alternatively look at other CAD programs like ViaCAD 2D/3D (which I have) or DraftSight which is very powerful 2D drawing for free, and very like AutoCad so many say - but was too complex for me.

PS  Having had a quick look at the manual I was not sure if NCCAD is CAD or CAM software.... it looks like it is possibly an integrated proprietry solution of both.  Good luck!

Edited By EtheAv8r on 16/08/2012 13:37:19

Thank you for the help so far guys.......

I purchased the ff500 direct from Proxxon, they have also offered very little help now I have purchased the machine!

To be honest I am quite enjoying G-Code as it's reasonably simple to grasp the basics.

There must be a way to import an .obj or .3ds model file and convert it to G-Code.

A little more info to my original problem.

I can create a model in Nccad easy enough but have no idea how to do the next step to simulate the cutting.

Thanks Jasmine x

There must be a way to import an .obj or .3ds model file and convert it to G-Code

That is done with a CAM program. Cambam is one of the lower priced versions :

http://www.cambam.info/

You can download an evaluation copy & use it 40 times unrestricted, then it hobbles to a limit of 500 lines of code. Cambam is not a full 3D program, but it does say in the blurb that it imports 3ds files. I have a copy but, as with many areas of interest, have not yet found the time to explore it's capabilities. I have had limited experience with OneCNC Mill Advantage at work - a combined Cad - Cam package that will import from other Cad programs or allow you to draw from scratch, convert to a machining strategy & post-process to produce a part program to suit most control formats. IIRC, our single seat 2 1/2D 3 axis package cost around £1300 (+Vat)

Other progams are available, but many of the full-feature industrial packages are priced outside the realm of most DIYers.

Out of interest, what are you wanting to make ?

HTH

Nigel B.

(edited to correct spelling mistakes - this editor is dire !)

Edited By Nigel Barraclough on 16/08/2012 19:44:47

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. 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

Right guys

Just got back from Paris and managed to get started on some G Code.

Starting off small and simple but, I keep getting errors, see below

When using NCCAD I get a Y Axis error at the first line......any ideas boys?

[IMG]http://i266.photobucket.com/albums/ii276/crash_photos_01/CNC_Help.jpg[/IMG]

;OUTER

G0 X-40 Y50

G1 X40 F400

G2 X50 Y40 J-10

G1 Y-40

G2 X40 Y-50 I-10

G1 X-40

G2 X-50 Y-40 J10

G1 Y40

G2 X-40 Y50 I10

;HOLE 1

G0 X-40 Y45

G2 Y45 J-5

;HOLE 2

G0 X40 Y45

G2 Y45 J-5

;HOLE 3

G0 X40 Y-45

G2 Y-45 J5

;HOLE 3

G0 X-40 Y-45

G2 Y-45 J5

;INNER

G0 Y-30

G1 Y30

G3 X-30 Y40 J10

G1 X30

G3 X40 Y30 I10

G1 Y-30

G3 X30 Y-40 J-10

G1 X-30

G3 X-40 Y-30 I-10

G0 X0 Y60

Third time lucky with the screen grab

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

Opps!!! This makes things go a little crazy.........

I guess this may have something to do with G2 & G3 being CCW & CW????

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

Thanks Terje

I am using......or trying to use lol Nccad 8.0 and tbh doesn't look as user friendly as 7.5

How would the depth of cut be controlled with a 2D project?

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

Hi Jasmine,

The screen dump seems to be of a simulator run from some G code that you have hand written. Your code looks ok to me; obviously the outer profile and the four holes are shown correctly. The move that seems to be causing the problem is:

G3 X-30 Y40 J10

The screen dump shows this move correctly, ie a CCW move starting at X-40 Y30 ending at X-30 Y40 with the centre of the arc at X-30 Y40. This means that your system is set to use absolute coordinates, with the I and the J values as incremental.

One slightly unusual aspect of your G code is that you have omitted I and J values when they are equal to zero, and X or Y coordinates when they have not changed since the last move. Some CNC controllers allow this some don’t; your simulator seems happy with this for all the outer moves and the four holes.

I would suggest you try the following on the offending line of code:

1) Explicitly set the I value to 0, just in case, ie.

G3 X-30 Y40 I0 J10

2) Erase the line and then re-type it, in case there are some non printing character embedded, or if you’ve used the letter o in place of the number 0. It sounds silly, but I have seen it happen often enough.

3) Check that there are no typos in the line following the highlighted line, or indeed in the rest of the program, sometimes the location the program stops at is not exactly where the error is located.

The error message is as helpful as most error messages are…. It will mean something to the programmer who wrote the simulator, but no help to anybody else!

You obviously understand G codes, so don’t be afraid to experiment, try different values and shorter program snippets until you find what is causing the error. As far as I can see there is nothing obviously wrong with the program you have listed.

Chris

Yippee finally cracked it

It appears that I needed to have both I & J values when using the G2 or G3 command even if they were zero.

I have actually managed to cut my very first piece today, thank you all so much

Here is the very simple G code, I have added ;descriptive help text so I don't forget what each bit does.

Opps just read your last post CC

You are spot on with your answer.

Thank you all so much.

J

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