3D design to CNC mill design flow

You might also look at G Simple - free to download CAM, can accept dxf input, or you can design simple things on-screen, it will generate and simulate g-code.

Hi Roger,

It wouldn't hurt to have Mach3 running unconnected. Whilst I'm not sure how much useful information you would get from it, I do think you would see glaring errors if you learnt to look for them. Mach has a toolpath screen that will give you an indication of how the tool is moving and also a table of maximum and minimum movements of X,Y & Z (very useful). The free version of Mach will be fine for this.

I'm not aware of any stand alone software that would display the part from G code and am not sure that I would trust one if there was such a thing. G code like any other language has dialects and it is often the little nuances that cause the problems.

One temporary solution, given your experience with steppers and servos would be to make a lash up machine which could be extremely crude given that it would be just to show how everything moves and check that nothing unexpected is happening.

Once you have reached a stage where the CAM program and Mach 3 are talking the same language the whole thing becomes very reliable and if anything stupid happens it will 99 times out of 100 be something you did.

David.

Plenty of advice, thanks everyone. I've followed up searches on just about every product and piece of terminology that has been mentioned, and I'm starting to connect the dots into a picture instead of a blur of information. Well, in theory anyway - I expect that practice will deliver the sound of misconceptions crashing to the floor.

In the blurb for various CAM programs the term 'post processors' comes up. I gather that these are to tailor the final output to match the requirements/idiosyncrasies of particular CNC machines. Fair enough, but this implies that there is an intermediate stage in the processing. Is that stage available as an output file, and is it in some standard format? Maybe plain vanilla G-code, or something else entirely? Is it useful?

One other question concerns detecting the extension of a tool bit after a change (or even at the start, for that matter). I guess one needs an electronic 'touch detector' at some predetermined spot within the workspace... I can think of a raft of questions surrounding this. Maybe someone could preempt them.

@David. Yes, it would be simple to hook up some steppers. Probably need some limit switches too, which means having the steppers actually move something, rather than just watching them turn. I think Mach3 is open-loop i.e. doesn't need feedback on position? (apart from limits).

I certainly have plenty to think about. Thank you.

Roger

I use NCPlot on almost every G-code program I generate. Since it creates the plot from the actual G-code it tells you what the tool is going to do, not what the CAM program thinks it is going to do. The toolpaths and material removal graphics you see in a CAM program are what the program intends to do, not what the G-code might end up doing. My CAM program doesn't always generate G-code that reflects what it thinks it is going to do. This seems particularly true for 4th axis programming, but I have had issues with 2.5D code as well.

NCPlot is also a useful sanity check against typos when G-code is hand written.

Andrew

Andrew

I'll have to check NC Plot out.

Roger,

For height setting I use a version of this **LINK**

For edge finding I use this type **LINK**

A better if not more expensive way is this **LINK**

The whole thing gets much easier the more you play with it.

David.

Another couple of minor points. NCPLot seems to be slightly more accurate on estimated machining time than my CAM program. The program also gives maximum excursions in all axes from the work offsets. That's very reassuring when the mill table is Z=0 and the work is mounted directly on the table. You definitely don't want to see Z minus.

Andrew

I have a little height setter which I built.

It has a magnet on the base that sticks it to the table; the silver circle you can see at the top is a spring-loaded tungsten carbide insert. On the right is a 4mm plug that connects it to the probe input to the controller. I have a simple Mach3 macro that, when the tool is positioned a few mm above the button, you click on "auto tool zero" on the programme run screen, it lowers the tool to the button, sets the tool height offset to 38.84 mm, then lifts the tool to 50 mm. I think the macro could be run from within a gcode program, but since I change tools manually anyway I just run it manually.

I have also made a little 10mm dia probe that fits in a collet, and has an isolated tip, with a macro that, run from the offsets screen, will locate an X or Y edge then set the work zero appropriately. I worked out a way to make sure the isolated tip is dead concentric with the shank, have been meaning to post it or write it up for MEW sometime.

Edited By John Haine on 16/12/2016 13:15:36

All useful info, thanks guys. I know that it was me who raised the question of tool height setting, but consideration of a couple of things in the replies, and all the further thoughts that they aroused, have led me to the conclusion that I'm going to wind up with a detail-info overload. They are obviously important factors that must be learned, but at the moment I'm still staring at an F360 screen and trying to remember which button to press next, so I'd like to leave this discussion for the moment, and return sometime later when my brain is ready to absorb a little more.

Thanks for all your help.

Roger