[Ed3XP]

Well, first let me introduce myself saying that I have very little experience with CNC and CAD work, but I am pretty computer literate and have been able to do ALOT so far with what I have to work with. I have a small (13x25) 3 axis Router machine (it was a DIY machine) with Mach3 It is a great little machine and very sturdy and has been doing alot for me! I also have access to Mastercam 4x. So here are the problems that I have run into so far and cant seem to fix. I have searched this forum and the internet, and I am still confused.

1. I make some code with mastercam and upload it into Mach3. I home the router to the top of the material (i place the bit right on the top). When I go to execute my code, it moves to the X,Y without first bringing the Z up to the "clearance". This causes some unwanted scars in my material. The clearance is set at .5 in Mastercam, and it works throughout the whole program, just not at start! Help me here!

2. When using contours in MasterCam, I select chain, and select the machine to route the "inside" of the chain. For some reason mastercam likes to ignore this, and it alternates between the inside and outside of different chains. So lets say I want to cut the word "CNC" out with contours, it cuts the Inside of the "C" while cutting the outside of the "N" and what not. This happens if I do it as one routine, or separate ones. This is quite annoying. I am using a 1/32 bit and there is plenty of room for the bit to fit. Especially since If I use the "Pocket" routine, it will do it perfectly! So I have been doing pocket and skipping to the final cut and let that run, but this shouldnt be!

3. Drilling holes! I am using adobe illustrator to make a simple part, Lets say a square with 4 holes by each corner. I make the circles in illustrator and make them 1/8" (and i use a 1/8" bit) and Then load it into mastercam, the circles (well everything) has a type of "line grid" inside of all the paths, and when I go to select drill, I have NO IDEA how to get it to select the inside of the circle I made in illustrator. Driving me nuts!

[ObrienDave]

Answer #1.

Your post is not outputting the "Z" clearance move 1st.
This will take some post modifications.
Pretty easy stuff there.

Easier fix is to MOVE the cutter up after you set tool length offset.
This is pretty much standard practice and easier than modifying the post.

Answer #2.

When selecting contours it is VERY important to select the PROPER direction.
For climb cutting, select the contour so it chains CLOCKWISE for the outside, and COUNTER-CLOCKWISE for the inside.
Reverse these rules for conventional cutting.
Yes you can change which side of the contour the cutter follows but unless you are consistant with which direction you pick them it can be confusing.

Pocketing will ALWAYS use the INSIDE of the most OUTSIDE contour.
This allows for pocketing with "islands".

Answer #3.

Most drawing programs like Illustrator, don't usually draw arcs as arcs.
They draw them as a series of closely spaced lines.
There is no actual "center".

The solution for this is to create an 3 point circle in Mcam using 3 of the line endpoints.
A better solution is to use Mcam's own CAD interface to create your part.

Good Luck,

[Ed3XP]

I will try the last two when I get home, about the first one....

When I zero out right on the material... I always lift the z up by a inch or so. When I hit run, it drops the z back to zero immediately before moving the X,Y. Is that what you are talking about? Or are you mentioning something else?

Thanks for the help!

[Ed3XP]

well answer 2 worked great!

Answer 1 is still the same issue, it zeros Z before doing anything else, so i gouge my material.

And for 3. i use illustrator to design all my stuff, the only thing I can see doing is just using the "pocket" tool to make my drill holes.. even though I dont like the idea. Gotta be a better way.

[John Bennett]

It is also possible to edit your error without changing everything by opening operation manager- click on "geometry" - "chain manager" opens pick the chain that is wrong (number 1 , 2 ,3 etc) -right mouse click and pick"change side" and then save.

[Ed3XP]

Anymore ideas on number 1?? It's a real bother

[mwoodard]

I am very new to all of this but have solved this myself the brute force way. I edited the gcode and remove the offending Z0 move that appears in the beginning of each gcode file. Now I have modified my post processor to eliminate that initial Z0 move.

Get rid of the Z0 in the line N104. I am sure that one of the experts will set me straight on this if I have remembered my early fix wrong.

Also, see that G8 command? It is a problem for Mach3. It puts the machine in exact stop mode which causes some real jerky machining. I edited that out also.


%
O0000(T)
(DATE=DD-MM-YY - 08-04-11 TIME=HH:MM - 08:55)
(MCX FILE - T)
(NC FILE - J:\MCAMX\ROUTER\NC\T.NC)
(MATERIAL - WOOD INCH)
( T1 | 1/4 STRAIGHT BIT | H1 )
N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N102 G8 P1
N104 G90 M05 Z0
N106 G52 X0. Y0. Z0.
N108 T1 M6
N110 G0 G90 G54 X-.0056 Y-.1542 C0.
N112 S18000 M3
N114 G43 H1 Z.25
N116 Z.1

[Excelmachine]

I am very new to all of this but have solved this myself the brute force way. I edited the gcode and remove the offending Z0 move that appears in the beginning of each gcode file. Now I have modified my post processor to eliminate that initial Z0 move.

Get rid of the Z0 in the line N104. I am sure that one of the experts will set me straight on this if I have remembered my early fix wrong.

Also, see that G8 command? It is a problem for Mach3. It puts the machine in exact stop mode which causes some real jerky machining. I edited that out also.


%
O0000(T)
(DATE=DD-MM-YY - 08-04-11 TIME=HH:MM - 08:55)
(MCX FILE - T)
(NC FILE - J:\MCAMX\ROUTER\NC\T.NC)
(MATERIAL - WOOD INCH)
( T1 | 1/4 STRAIGHT BIT | H1 )
N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
N102 G8 P1
N104 G90 M05 Z0
N106 G52 X0. Y0. Z0.
N108 T1 M6
N110 G0 G90 G54 X-.0056 Y-.1542 C0.
N112 S18000 M3
N114 G43 H1 Z.25
N116 Z.1

I've never run a router before but why do you have G52 on line 106?

[jolafson]

I would bet that you have the wrong post for your machine/control. I've seen a few machines that the first lines of code contained a G91 G28 Z0 to take the spindle straight up to Z home position, then tool change, position etc...

As for the G52, It is telling the machine to go to home position before excecuting the tool change. You can set up your control def. or post to send the machine home before each tool change or just retract the head.

[Ed3XP]

Thanks! I have no idea how to edit a post, but I'll try to figure it out