[cubby]

This is what it Looks Like,
I know I'm Doing something wrong, But have tried for three days to make this work,
Program support is useless as tits on a boar hog!!
cubs

[Jim Dawson]

Not sure what problem you are having, no explanation in your post. But what I do see is the rapid move speed is set to 0.0000, nothing is going to move because a G00 (rapid) is the first move in the G code.

[cubby]

Jim, I am Sorry this is from another thread, I didn't know how to post the pictures and had to start another thread to post the pictures,
cubs

[the_gentlegiant]

Jim, I don't even know you but I know you know better. Rapid moves are never programmed with a feed rate. The machine decides that along with the setting of the feedrate over-ride dial.

What I see are two things. I have no idea what software this is so I'm going only by what's in the pictures.

1) You have the box checked that causes you to be programming On The Line. In this mode you would need to be using Cutter Compensation, otherwise in your current state, your circle is going to come out 2 1/4" diameter instead of 2". I see no button for Compensation, and your code doesn't show any turning on and off of Compensation. (G41/G40) In general I suggest Left Of Line. If a bore you want to cut CCW with Path To Left. (G03) If a boss you want CW with Path To Left. (G02) In both instances this will cause climb cutting, which is generally what you want.

2) Your program is not outputting a J coordinate (Incremental distance from arc center including sign in Y) Try adding J0. to your code and see if that helps.

3) You realize you're cutting out a circle and leaving a plug in the middle. This is okay in your piece at it seems you're only going 1/4" deep. This is not a good strategy on thicker material. You either first need to drill out most of it, or helical machine it out, turning all of it into chips. On thicker material, unless you're running thru tool coolant or have very good flood and perhaps a high helix tool, the cut groove will get too deep to realize effective chip removal. Plus when a big slug breaks free it can sometimes cause problems like chipped cutters.

4) Endmills hate plunging. Try pre-drilling a hole where your tool is starting. That or ramp your 0.075" from the center to the cut diameter, cut the circle at that depth, and then move back again to the center for every depth. Your cutter will love you for that. If you're running aluminum with a very short flute length tool, you'll likely get away with what you're doing in plunging. Just not best practice.

Hope this all helps.

[machinehop5]

...is this the Program you using...you forgot to post it in this thread
Intuwiz G-code Generator

[cyclestart]

Sorry but I have more questions than answers.
What cnc control ? Mach, grbl, other ?
That code would moves the spindle a complete 360 degree 2" circle on my control but it may not on yours.
On my control relative incremental arcs are default but your control may need setting to that.
As mentioned by gentle_giant your control may expect J or an X for G2/G3, it will be in the control manual(?).
Apologies if you mentioned control name and I missed it.

Edit/machineshop 5 faster on keyboard

[Jim Dawson]

Jim, I don't even know you but I know you know better. Rapid moves are never programmed with a feed rate. The machine decides that along with the setting of the feedrate over-ride dial.

Normally I would agree with what you said, but in this case it looks like the rapid speed is programmed in the G code or set up in the CAM. Never seen that before. But I have no idea what the control system is, so I can only make a best guess.

[cubby]

Ok Fellers, Mach3 is my controller,
Ok I found an ON LINE G-code app, I entered all my information and Entered the code into a PC I have here That I am building up for another CNC. It has Mach3 already installed,
I wanted to run this code in simulation and see what it looked like,
Low and Behold it Looked JUST LIKE it was supposed to Look. I was Watching the Z-Axis Numbers as it was Simulating the cut. It Started at X-0 on Left. Moving Clockwise toward the top, When it got to the top it had got to ONE INCH, "Hence" Halfway to the other side of X-axis,
It all Looked good, I put the code on a thumb drive and went to my shop, Loaded it, "SAME CODE" and it looked like a 3/4 Wash Tub Circle, GIANT CIRCLE,, On First Computer it was very small on the screen. As it Should have been a 2 inch circle, I'm Posting this Code,

G20 (inches)
M6 T1 (Change Tool: Diameter: 0.2500 in)
M3 (Start Spindle)
M7 (Flood Coolant On)
G0Z1.0000
G0X0.0000Y0.0000Z1.0000
G0 X0.1250Y1.0000
G1 Z-0.0250F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.0250
G0 X0.1250Y1.0000
G1 Z-0.0500F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.0500
G0 X0.1250Y1.0000
G1 Z-0.0750F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.0750
G0 X0.1250Y1.0000
G1 Z-0.1000F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.1000
G0 X0.1250Y1.0000
G1 Z-0.1250F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.1250
G0 X0.1250Y1.0000
G1 Z-0.1500F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.1500
G0 X0.1250Y1.0000
G1 Z-0.1750F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.1750
G0 X0.1250Y1.0000
G1 Z-0.2000F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.2000
G0 X0.1250Y1.0000
G1 Z-0.2250F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.2250
G0 X0.1250Y1.0000
G1 Z-0.2500F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.2500
G0 X0.1250Y1.0000
G1 Z-0.2750F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.2750
G0 X0.1250Y1.0000
G1 Z-0.3000F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.3000
G0 X0.1250Y1.0000
G1 Z-0.3250F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.3250
G0 X0.1250Y1.0000
G1 Z-0.3500F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.3500
G0 X0.1250Y1.0000
G1 Z-0.3750F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.3750
G0 X0.1250Y1.0000
G1 Z-0.4000F5.00
F5.00
G2 X0.1250Y1.0000 i0.8750j0 z-0.4000

[ger21]

The IJ mode on your two versions of Mach3 are different. Change them in General Config.

[cubby]

The IJ mode on your two versions of Mach3 are different. Change them in General Config.

In Config settings,, What Setting is it Ger?
Also, Is it possible to set up Inches and Millimeters on one machine?
Thank You
cubs

[machinehop5]

I know I'm Doing something wrong,

View from here looks good. CAD/CAM programming is hard to learn/do...it has to be perfect or the machine doesnt play.

[cubby]

View from here looks good. CAD/CAM programming is hard to learn/do...it has to be perfect or the machine doesnt play.

Yes it is evident now as what Ger said about a setting being wrong with the I and J mode,
But I'm not smart enough to find those settings he is referring to, Will do some more reading, The Square Holes I just do by hand, And I have cut one Round hole by hand,
But is very time consuming, Where as the mill can do it in just a few minutes, Trying to Mill all the Motor plates and Gantry's for a New machine, . I'm Like the Blind Leading the Blind, LOL
cubs

[handlewanker]

Hi, I was under the impression that if you wanted to cut out a large diam circle with a centre plug you went round the circumference and left a few tags to hold the centre bit up.....correct me if I'm wrong.

I'm still very much a CNC G code learner but a few things in the code sequence in post #8 seem out of wack to me:-

In line #5 you have G0......why is the G0 in line #6 and #7 as well....Isn't G0 modal?

Also, line #6 has X and Y values as zero with a Z value at 1.0000...…..why do you need to have the X and Y values in that line?

In line #8 you have a F feed rate value as 5.0.....and in line #9 you repeat the feed rate vale as 5.0...….am I misunderstanding the code sequence?

I'm very pedantic when it comes to formal G code writing....because I learned that way from people who know...….the code should start and end with % and a program number...……...having the N sequence for code line numbering makes identifying the line visibly easier......am I wrong in this assumption?
Ian.

[cubby]

Hi, I was under the impression that if you wanted to cut out a large diam circle with a centre plug you went round the circumference and left a few tags to hold the centre bit up.....correct me if I'm wrong.

I'm still very much a CNC G code learner but a few things in the code sequence in post #8 seem out of wack to me:-

In line #5 you have G0......why is the G0 in line #6 and #7 as well....Isn't G0 modal?

Also, line #6 has X and Y values as zero with a Z value at 1.0000...…..why do you need to have the X and Y values in that line?

In line #8 you have a F feed rate value as 5.0.....and in line #9 you repeat the feed rate vale as 5.0...….am I misunderstanding the code sequence?

I'm very pedantic when it comes to formal G code writing....because I learned that way from people who know...….the code should start and end with % and a program number...……...having the N sequence for code line numbering makes identifying the line visibly easier......am I wrong in this assumption?
Ian.

Brother, That is the Way that the App wrote the code with the information that I put into the System,
We all know that there is NO RIGHT Way to write code, There are many ways in achieving the same result.
I qant to be able to write what I want the machine to do also, But that takes lots of reading and hands on,
cubs

[the_gentlegiant]

Hi, I was under the impression that if you wanted to cut out a large diam circle with a centre plug you went round the circumference and left a few tags to hold the centre bit up.....correct me if I'm wrong.

I'm still very much a CNC G code learner but a few things in the code sequence in post #8 seem out of wack to me:-

In line #5 you have G0......why is the G0 in line #6 and #7 as well....Isn't G0 modal?

Also, line #6 has X and Y values as zero with a Z value at 1.0000...…..why do you need to have the X and Y values in that line?

In line #8 you have a F feed rate value as 5.0.....and in line #9 you repeat the feed rate vale as 5.0...….am I misunderstanding the code sequence?

I'm very pedantic when it comes to formal G code writing....because I learned that way from people who know...….the code should start and end with % and a program number...……...having the N sequence for code line numbering makes identifying the line visibly easier......am I wrong in this assumption?
Ian.

Good point about the plug tabs. That's certainly a way to do it. But then you have to deal with breaking out the slug and finish machining the tab areas. In a production setting where you want to remove finished parts out of the machine, stopping to knock out and remove plugs, then restarting the program to clean off the tabs, do a finish pass and perhaps chamfer the bottom of the bore is not a good strategy. Also it is very difficult to get proper chip evacuation out of deep slots you may be creating cutting out say a one inch deep plug with a 1/4' tool. Another problem is you'll still have to go back in for a finish cut because no way you will end up with a nice finish in a slotted out bore.

Glad to hear of you G code training. Seems to be a dying breed. Like you, trashy G code gets under my skin. There are many post processors that put out crap compared to what I put out semi-manually. And seems few people take the time to fine tune their posts to not put out crap. Part of that problem is because many users don't know what good G code looks like. What you see above is typical if you ask me.

For almost all occasions I find line numbers a total waste. You need them in parts of lathe routines and here and there in subroutine calls, but other then that they only take up space. I completely disagree that they make things easier to read. To me just the opposite. Memory is lacking and expensive on older controls. Line numbers eat up tons of memory. So do repeated Modal calls. I will say that line numbers help here when discussing programming online in forums, but other then here, people aren't generally talking over long distances with others about their programming, so no numbers needed if you ask me.

Finally - the % sign is likely not needed for all controls. What you described is typical for Fanuc controls, but I doubt every control uses them or O prefixed program numbers. I could be wrong but...

Sorry cubby. Don't mean to hijack your thread. Just borrowed it for a minute. Hope you don't mind.

[machinehop5]

3.141...is just a number 29th Feb 2020

[routalot]

Am I the only one to note the absence of a G20 or G21?

I also like line numbers,if you have half a million lines of code it gives an idea of how much further you have to run.On a large 5 axis job I had 188 million lines to get through.Never seen more that 740,000 on my home machine though.Its really handy if you have an electricity supply subject to occasional interruptions as you can make a note of the line numbers every ten minutes or so and if the power goes,you can resume without losing too much time running the whole sequence.

In the case of this particular problem I think I would recommend an hour or two learning Fusion 360 as the supposedly intuitive software isn't living up to the description.I presume it doesn't have a simulation function as that normally shows up things that won't work.If learning Fusion seems like a mountain to climb,perhaps downloading Camotics for a simulation would be useful although I have found it rather slow.

[handlewanker]

I liken G code to writing a page of text......you can leave out all the punctuation, capital letters, full stops and commas etc and still be able to read the text.

I've found that Mach3 will still move the tool without many (some) of the parameters that are written......but at the same time I wouldn't go to sea in a small boat without a lifejacket even if the boat was seaworthy.

I'm just too new at CNC to really argue a point...…..so far I have not needed to entrust a work plan to a CAM program as I am learning and just having a fun time working out how a tool moves and the plan I write to make it do it without a drama.
Ian.

[the_gentlegiant]

I'm just too new at CNC to really argue a point...…..so far I have not needed to entrust a work plan to a CAM program as I am learning and just having a fun time working out how a tool moves and the plan I write to make it do it without a drama.
Ian.

It's obvious everyone has their own ideas and needs with line numbers. Though most software and machine controls have settings or parameters that can turn on or off automatic line numbering. So obviously the people who make these things understood the different needs. Mostly people running older Fanucs with limited memory will appreciate the memory savings of leaving line numbers where they belong. Like not there. :-) Ha... sorry.

handlewalker I wish everyone took the time to do what you're doing. Even if someday you end up on a high end CAD/CAM system, knowing what the CAM spits out and being able to clean up and correct it makes you a much more skilled and hence desirable operator.

I would not try to steer clear of CAM completely. I program manually on 18 year old CAD/CAM software. My shop doesn't run into 3D 5 axis stuff so that's not an issue. But when writing G code sentences, manually entering X - Y and Z coordinates is something the CAM should be doing for you always. Typing in coordinates is very time consuming and totally prone to errors. And make no mistake, a single misplaced period or missing - sign or any number of things can potentially cost thousands in an instant when it creates a machine crash. That's another thing about you learning to read and understand G code. When you're standing at the machine single blocking a first run on a part, you'll be able to look at the next line the machine is going to operate to, and understand exactly what the machine is about to do before it does it. I can't tell you how many times I've stood there and thought... oh that's not going to work, and hit Reset to go back and correct the problem before it causes trouble. Even with Simulation software, some of which can be poor at best, knowing what you're reading will never hurt.

Sorry cubby... I'm dong it again. Damn. Though I think I"m done. :-)

[cyclestart]

This isn't CAM software with selectable post processors etc.
It's more like a 'g-code helper' and a user will need to know what edits are necessary (or beneficial) for their control.
It would be possible to string together a complete part program using the various routines but it lacks the niceties included in CAM. For example ramping and 'roll around sharp corners' and just generally strategies that are kind to both tool and machine. I will still hand code when CAM isn't practical (ie: want to cut this NOW) but otherwise CAM all the way.

Like routalot I suggest looking for CAM software. Also learning the basics of g-code is a genuine good thing.