Need guidance on manual tool changing best practice (and other things)

Hi everyone, so far doing fine running the cnc and trying to practice more, I have thought about it but not yet practiced this process because I feel it would need a lot of trial and error and I'm trying to minimize that with your guidance.

first background:
I built my machine recently ( http://www.mycncuk.com/threads/8334-...ewbie)?p=66167 ) and so far so good with cutting alu and wood. of course I'm far from best setup and all but it is acceptable heh.
Spindle is 2.2kw ER20 collet so I have to manually change the tool if I want to use more than one for the operations on the work piece.
I also have a simple probe for auto Z height and it works with a macro I got from the net wonderfully.

now I have a couple of questions:
-first most important question. at the moment I'm using solidworks and HSMExpress, in that software I can setup the tool library and select the endmill size, type and etc that will do the operation, that of course is necessary to produce the correct G-Code. but I'm a bit confused because I see in the commercial machining center software control you also maintain the tool information. so my question is why do they maintain the information on the machine computer if the G-Code was already adjusted at design stage? aside from pre-storing the actual tool heights so that the machine can figure the starting depth I'm not sure the process flow.

-since my machine is DIY I figure in order to do a job with multiple bit setup is just a matter of pausing at tool change M code and manually replacing the bit and then setting the zero Z again (maybe??) and resume. assuming I put the correct tool size and changes in the G-Code and the cam software modified based on that and all. is this the correct way or am I missing something?

-for parts that need machining on multiple sides what is the process here? for example do we machine one face and make sure the shape that comes out can be clamped so that we can put it upside down and do the other one? do we probe the edges and set something in mach3? I know the answer might not be straight forward or easy but just a bit of pointers from you guys I'm sure I can understand much faster than trying myself.


thanks so much and appreciate any comments, as always.

Lots of questions, but just thinking about the tool-table thing - one reason is that you can generate gcode with a toolpath where the the CAM software knows tool diameter and offsets the toolpath by tool radius, or the toolpath follows the centre-line of the cut and the motion control software uses local tool data to generate the offset on the fly, so to speak. One advantage of the second approach is that you can change tool size without needing to regenerate the gcode, or more likely you can tweak the tool table numbers to allow fine adjustment to cope with tool sharpening or tiny variations in tool size if you change cutters. For home use, I can rebuild the gcode very quickly if I need to make tool size allowance, but commercially where the guy running the machine can't or shouldn't change gcode but still needs to recalibrate for tool changing, the local tool table makes sense.

Tool tables in the CAM software are fine if you use repeatable tooling and have the same numbers programmed into the Mach3 tables. I see much danger if the CAM spits out a H204 (height offset for tool 204) and it crashes through your part, table or worse. So for you keep the tool table in Mach3 clean and make sure there are 0's everywhere. Some CAM programs will put a description comment in the code to tell you what each of the called tools is. This is useful so you know which one to select next. You will need to re-zero the height each time manually.

Toolchanges are called using an M6 code. You will need to tell mach to stop at these in general config. M6 allows you to move the head in all axes so you can touch-off. If you set up a touch off plate you can do this automatically.

I would suggest you look up Ger21's mach3 screen (Mach2010) on here, CNCzone and youtube. It will make life much easier and is worth every penny. Just remember to keep all the tool table values set to 0.

http://www.machsupport.com/forum/ind...c,17004.0.html


For the two sided machining you have the answer already. It is all about making fixtures to ensure you can flip the part over and find x0, y0 again for that face. You can use dowel pins, rails or whatever else. Plenty on Youtube to keep you learning.

Regards

George