Manual Numerical Control - 'CNC' done by hand with a DRO

[Roger]

This thread explores the possibility of using CAD to create tool paths which can be used on a manual milling machine which has a DRO

In CNC you treat the job as if it were laid out on a piece of graph paper with the origin being your X0Y0 position which is anywhere convenient. It doesn't matter where, so long as you can set the mill to it. So it can be a corner, the middle of the job (found with a wobbler from both sides) or a hole.

That means your X and Y coordinates can go plus and minus if you like. All that matters in CNC is that you only have one zero point. You set that in the CAM program and that means that the G-Code will all be relative to that.



This is how a simple drill output is shown using the Alibre Design CAM module. It's pretty much the same whatever CAD/CAM you use.
Here you can see there are two triads (zero arrows). One is the origin of the CAD model, how it's been drawn, and the other has been set to the centre of the job in X and Y. That's the one that decides what the G-Code is output from

Narrow step drilling by Roger Froud, on Flickr

So a G-Code output would have a series of commands to indicate it's a drilled hole for example, and the X,Y coordinate where that's going to be. Nothing more than that.... repeat until it's all done. The beauty of this approach is that you set the datum once and then forget about it. It's either all right or all wrong!


This is the raw G-Code that my system outputs for that. You can see it tells you what the tool number and size is, the spindle speed and three lines for each drilled hole that most CNC systems recognise. Don't take any notice of the Z-12.654 values, I don't use the machine to drill holes automatically when there are only a few holes so I don't set all of the values.

(4 holes)

(Tool Dia. 1.4 Corner radius 0.7)

T4

S1000M03

G01 X13.500 Y7.160 Z6.000 F1000.0

G81 X13.500 Y7.160 Z-12.654 R2.500 F30.0

G80

G01 X13.500 Y7.160 Z6.000 F30.0

G81 X4.500 Y7.160 Z-12.654 R2.500 F30.0

G80

G01 X4.500 Y7.160 Z6.000 F30.0

G81 X-4.500 Y7.160 Z-12.654 R2.500 F30.0

G80

G01 X-4.500 Y7.160 Z6.000 F30.0

G81 X-13.500 Y7.160 Z-12.654 R2.500 F30.0

G80

G01 X-13.500 Y7.160 Z6.000 F30.0

M5M30

I've written a little utility program that rips out all that stuff so it ends up looking like this....

(4 holes)

(Tool Dia. 1.4 Corner radius 0.7)

T4

S1000M03

G01 X13.500 Y7.160 F1000

G01 X4.500 Y7.160

G01 X-4.500 Y7.160

G01 X-13.500 Y7.160

M5M30

On my machine, that allows me to single step from hole to hole, each G01 is a move to the next point.

Just to make this crystal clear. The idea is to turn the handles on the mill until the DRO shows the the positions shown in the list. You don't touch the DRO once it's set to the job zero.

These hole positions can be used with a DRO from a single datum to drill all of these holes.

I'm sure many of you are thinking this is an awfully long way around the houses to do something that you could easily have worked out in seconds on the back of a fag packet, but look at the bigger picture. This is a trivial example, imagine 100 holes on a frame, with all of the coordinates listed for you, grouped neatly into the different tool sizes. Now that has to be appealing!

Also imagine the possibilities of using the outputs to tell you where to move a milling cutter to machine a profile as in a 'part on a stick'. As long as you're machining straight lines, that's a trivial exercise. If you need to generate more complex profiles, you can generate outputs with many straight lines if you don't mind moving between all of them to generate the desired shape!

I think this method has huge potential without going to full CNC.

[Deleted]

Thank's for starting this thread Roger..I'll try to digest it a little but will probably get much further into understanding things once I have a DRO in front of me that can do this. I find doing things myself in practical terms, is the best way for my brain to take in what's what...I'll follow what's said in this thread very closely...

cheers

Pete

[Roger]

Aug 31, 2018 10:05:18 GMT @greenglade said:

Thank's for starting this thread Roger..I'll try to digest it a little but will probably get much further into understanding things once I have a DRO in front of me that can do this. I find doing things myself in practical terms, is the best way for my brain to take in what's what...I'll follow what's said in this thread very closely...

cheers

Pete

Hi Pete,
I too find that doing it myself is by far the best way of learning. As a toddler, I'm credited as saying "self do it" when others wanted to baby me. Ever since, I've been called a "self do it"... and forever shall it be so!

Once you picture your machine as just an X/Y plot looking from above, the rest falls into place. Any Z values are just changing the height. Those things are probably less useful in MNC, but they might still have their uses.

[Roger]

I'll take a look at profiling next. I see that Lisa is machining port faces, and this is just the sort of thing where this approach can make life a lot easier.

Watch this space...

[runner42]

Hi Roger,

a pre-requisite is having CAD/CAM software, the CAM element generates the G code so CAD only software isn't any good. For those who have CAD/CAM software how the G code is outputted is self evident, would however for those without CAD/CAM benefit from a few words on how this is generated? In your utility program you no longer require to specify the Z axis readings because drilling on a manual milling machine you operate the handle until (in this example at least) the drill passes through. But in your to follow example ie port faces the Z axis element would need to remain.

In any following listing of (software) steps is it possible to add comments of what each line is doing for the benefit of those interested but not too savvy readers.

Brian

[Roger]

Sept 1, 2018 7:25:27 GMT runner42 said:

Hi Roger,

a pre-requisite is having CAD/CAM software, the CAM element generates the G code so CAD only software isn't any good. For those who have CAD/CAM software how the G code is outputted is self evident, would however for those without CAD/CAM benefit from a few words on how this is generated? In your utility program you no longer require to specify the Z axis readings because drilling on a manual milling machine you operate the handle until (in this example at least) the drill passes through. But in your to follow example ie port faces the Z axis element would need to remain.

In any following listing of (software) steps is it possible to add comments of what each line is doing for the benefit of those interested but not too savvy readers.

Brian

Hi Brian,
You're quite right about CAD on its own not being enough. However, Fusion360 is free to modellers at the moment and that has CAM integrated into it. Unfortunately, I can't give examples of how the G-Code is output using that because I use Alibre Design with Mecsoft's CAM module which is different.

Suffice to say that the creators of this software try to make the process as simple as possible and there are YouTube tutorials about Fusion360 if you want to see exactly how it's done.
There are way more controls than you need, especially since there's no need to generate any of the entry and exit moves when milling for example. You also don't need to output G-Code that progressively takes cuts along the same path at different depths since you can control this yourself and repeat a simple series of moves.
So for the port faces example, the only Z value I'd want to be left in would be for the final depth.

I'll certainly comment the lines of the following examples. Most G-Code outputs include a load of superfluous junk at the beginning of every program which is confusing when you first start. This code assumes that the machine has been left in a completely unknown state and attempts to set everything up every time it's run. I've ripped all that stuff out from the post processor in my system so I get the nice clean output that I've listed.

[Mike Clarke]

Hi Roger,

Nice! I'd never thought of this - previously I have just printed off a dimensioned drawing and calculated cuts/hole positions manually from it. This will be a very handy technique and avoid easily made errors.

I've never even looked at G code before......but had a play on Fusion360 this afternoon (have to admit spending half an hour with a cuppa watching simulated machining!!).

Thanks for sharing.

Mike - saving up for a CNC setup.

[Roger]

Sept 1, 2018 16:05:51 GMT Mike Clarke said:

Hi Roger,

Nice! I'd never thought of this - previously I have just printed off a dimensioned drawing and calculated cuts/hole positions manually from it. This will be a very handy technique and avoid easily made errors.

I've never even looked at G code before......but had a play on Fusion360 this afternoon (have to admit spending half an hour with a cuppa watching simulated machining!!).

Thanks for sharing.

Mike - saving up for a CNC setup.

Hi Mike,
I think it's been overlooked, I've not seen it done before. The benefits of CAD can greatly be extended if you can use that data to generate useful coordinate date.
The next step is to show how you can profile to a rough dimension using the CAM output and then finish to a new set of coordinates that take you spot on to size. That's really useful too, and it's the way it's always done with CNC, but a pain to work out by hand.

[Roger]

This is a simulation of a single port in a cylinder for the purpose of this next example.

I ought to make absolutely clear that this assumes you have linear scales that measure the actual position of the table. This won't work if you're using the dials or a DRO that measures the angular position of the leadscrew. Backlash is assumed to be zero!

You can see that I've put the origin Triad at the top centre of the slot. This would be the same even if there were additional ports on either side. It all comes out in the wash, you wouldn't move the zero for each slot.

So on the cylinder block, you would use a wobbler for example to touch the LH end, then click to zero the X DRO
Then move to the other end and use the wobbler to find the RH end. Halve the reading on the DRO and set that as the current position.

Do the same for the Y axis

Block by Roger Froud, on Flickr

I defined 5 x 2.5mm holes at 2.9mm centres to remove the bulk of the material. Only one is necessary really, you can mill out the rest, but I've done this because it's typically done. The slot is 3mm wide.

I've used a Drilling Operation and told it to use the sketch of the 5 holes as the source.

The output shows Red lines for the high speed moves clear of the work and Blue lines which is the path of the centre of the drill.

The Orange lines are just to show what it is we're machining. The depths don't matter because we just want the centre coordinates from the program.

Pilot holes by Roger Froud, on Flickr

This is the output from the CAM program. 

(Pilot drill)
    -  Anything in brackets is a comment.
(Tool Dia. 2.5 Corner radius 1.25)
    -  I've configured the Post Processor to output this for me.
T2
    -  Each tool can be assigned a number
S1000M03
     - S1000 is the RPM and M03 turns on the spindle.


- new lines added for clarity


G01 X0.000 Y-5.800 Z6.000 F1000.0
    - Go to X0Y-5.8 with the head up at 6mm at a feed of 1000mm/min
G81 X0.000 Y-5.800 Z-12.972 R2.500 F50.0
    - Then the CNC control would interpret this to go to Z-12.972 which is not needed
G80
    - This signals the end of drilling

G01 X0.000 Y-5.800 Z6.000 F50.0

G81 X0.000 Y-2.900 Z-12.972 R2.500 F50.0

G80


G01 X0.000 Y-2.900 Z6.000 F50.0

G81 X0.000 Y0.000 Z-12.972 R2.500 F50.0

G80


G01 X0.000 Y0.000 Z6.000 F50.0

G81 X0.000 Y2.900 Z-12.972 R2.500 F50.0

G80


G01 X0.000 Y2.900 Z6.000 F50.0

G81 X0.000 Y5.800 Z-12.972 R2.500 F50.0

G80


G01 X0.000 Y5.800 Z6.000 F50.0

M5M30
- Turn off the spindle and rewind the program

... and this is what that looks like cleaned up by my utility program. You don't have to do this of course, you can use the raw output but this is easier to read.

(Pilot drill)

(Tool Dia. 2.5 Corner radius 1.25)

T2

S1000M03

G01 X0.000 Y-5.800 F1000

G01 X0.000 Y-2.900

G01 X0.000 Y0.000

G01 X0.000 Y2.900

G01 X0.000 Y5.800

M5M30


So you can just go to those coordinates and drill the holes there. No need to mark anything out.

This is the profile as if we were using a 1.5mm cutter. It doesn't matter for this example what size it is as long as it's smaller than the slot plus the amount of stock we've told the CAM operation to leave, which in this case is 0.2mm

I've told the CAM operation not to generate any entry moves, I just want the corner coordinates of the centre of the tool. With CNC, I always use the centre of the tool, it's less confusing in my opinion. Obviously that's the only choice if you're doing this by hand.

Again, the Blue lines show the centre line moves of the cutter and the Orange is what we're cutting.

Rough slot by Roger Froud, on Flickr

The CAM output for the roughing operation, leaving 0.2mm of stock, is this...

(Rough profile)

(Tool Dia. 1.5 Corner radius 0.75)

T1

S1000M03

G01 X-0.550 Y6.550 Z6.000 F1000.0
    - Move the tool centre to this X/Y position with the head up at 6mm
G01 X-0.550 Y6.550 Z-1.000 F300.0
    - Repeat that position but put the head down. 
G01 X-0.550 Y-6.550 Z-1.000 F50.0
    - Now move around the profile coordinate by coordinate.
G01 X0.550 Y-6.550 Z-1.000

G01 X0.550 Y6.550 Z-1.000

G01 X-0.550 Y6.550 Z-1.000

G01 X-0.550 Y6.550 Z6.000 F1000.0

M5M30

Ignore the Z figures, you would go around the perimeter, taking the same cuts you normally would until you get to the depth you want.

You'll notice that every line has X,Y and Z which is unusual. This is because I've configured the Post Processor to do that. It makes what's going on clearer in my opinion and helps if you're restarting a program part way through.

Obviously you don't need to slavishly follow this program, you're going to want to drop the tool into one of the drilled holes first and then start following the coordinates.

After this roughing cut, the slot should be 0.4mm under size because we told the CAM operation to leave 0.2mm stock all round. You then measure the width and check that this is correct. If it is, copy the CAM operation to make a new Finishing one, and change the stock to zero. This will prevent the output overwriting the roughing program, you will probably have two of these to do!
If the size is wrong, adjust the amount of stock so that the next cut will take it to the right size. Remember that it's the stock you're leaving on BOTH sides so you need to correct for half the amount.

This is the output I got for that operation. You can see that the output is 0.2mm further out for each move.

(Finish profile)

(Tool Dia. 1.5 Corner radius 0.75)

T1

S1000M03

G01 X-0.750 Y6.750 Z6.000 F1000.0

G01 X-0.750 Y6.750 Z-1.000 F300.0

G01 X-0.750 Y-6.750 Z-1.000 F50.0

G01 X0.750 Y-6.750 Z-1.000

G01 X0.750 Y6.750 Z-1.000

G01 X-0.750 Y6.750 Z-1.000

G01 X-0.750 Y6.750 Z6.000 F1000.0

M5M30


So that's it really, it's pretty simple and you can use the same method when there are more slots, all of the operations being grouped together for each slot if you want.

The beauty of this method is that you don't need to keep measuring and working out whether the cuts are in the right position to each other or some other datum. You can mark it out if you want and check by eye that you're happy it makes sense for the diameter cutter you're using before you take a cut.

One last point... the cutter is always the thing that moves in CNC, regardless of whether the table or the spindle moves. X moving more +ve always moves the cutter to the right on the machine if you're looking down on the job. Knowing this means you're never guessing which way to turn the handle!

Clearly you can use this method on outside profiles, but you would need to make sure the CAM output doesn't roll the cutter around the corner which is the default. If you don't do this, you will get lots of commands to generate an arc on the corner which is not what your want.

You can see what all the G-Codes are here, Fusion360 will output loads of them by default at the start of each program.

I ought to mention what a Post Processor is too. Each CNC machine has it's own dialect of G-Code which reflects the evolution of the language and machine in question. Each CAM program comes with a huge library of these, hopefully one is suitable for your CNC machine! I selected the one with the simplest output and then edited it so that it formats the output the way I like it.
So in a nutshell, it's like the CAM program only knows Esperanto, but it can translate that into English, Spanish etc to suit the machine it's aimed at.

[silverfox]

Roger
Seen your other post directing us here.
It may take some time (like learning Chinese!) but i think i might get there without the expense of buying a CNC machine!!!

IF you take a right angled triangle as an example ABC with the hypotenuse being the line BC i can frasp the concept of cutting AB and AC but the BC bit will need working on. A machine will move both axis a smidgen to get the line right, but how a human does it
The same with radii
Still it will be fun filling the scrapbox!
Have a look at a B17 radius rod to see wht i mean!!!

ron

[Roger]

Sept 1, 2018 22:38:26 GMT silverfox said:

Roger
Seen your other post directing us here.
It may take some time (like learning Chinese!) but i think i might get there without the expense of buying a CNC machine!!!

IF you take a right angled triangle as an example ABC with the hypotenuse being the line BC i can frasp the concept of cutting AB and AC but the BC bit will need working on. A machine will move both axis a smidgen to get the line right, but how a human does it
The same with radii
Still it will be fun filling the scrapbox!
Have a look at a B17 radius rod to see wht i mean!!!

ron

Hi Ron,
You've spotted the big problem with MNC, it's painful moving dozens of tiny increments to create even a simple straight line at an angle. This is where the computer comes into its own.

I'm not really advocating this method for creating complex shapes that depart from straight line moves in one axis at a time, it's too time consuming. Having said that, it is possible, and the alternatives aren't that attractive either.

However, I think it's a valuable method for creating orthogonal shapes with holes in them. Most people won't have ever used the 'part on a stick' method, and this offers a way of machining around a profile or slot without repeated setups and worrying about backlash. This change in mindset is the gateway to CNC machining.

[silverfox]

Roger

Off to Soton in about 10 mins to see a few 'big ships' and ride on the Hythe Tramway.

Will put my Worsel Head on when i get back. ( its nice to know i am 'sort of' grasping it, even though it may not be the clean end of the stick)

Ron

[doubletop]

Whoa! I think this thread needs a reset.

Roger has picked up my “MNC” concept but started at MNC 103 when we really need to start at the beginning. CAD is unnecessary to be able to use your DRO’s to do MNC. Most DRO's do the maths for you so I think we need to build up the concepts for everybody, look at the functions DRO’s provide and later introduce CAD and the G Code outputs.


So off the top of my head we should be looking at

• Drawings and the types of machining operations we may want to perform.
  
• The macro functions DRO’s provide out of the box.
• Establishing datums and reference points necessary to perform those operations by using basic trigonometry.
• 2D CAD to get the datums and reference points.
• Extending the concepts with 3D CAD and G Code.

In my case MNC is something I have had in mind to write up for a few years now, only recently have I been using CAD to inform my work as I was doing a more complex project. I had been meaning to write this up for ME and had discussed doing this with Dianne Carney. But now the cat is out of the bag lets get on with it. Maybe in the long run Roger and myself can write it up more formally and get it published?

By way of a taster here is a simple job just using the DRO's no CAD whatsoever,

And a more complex job where CAD was neccessary

Pete

[Roger]

I suppose it depends on how much work you want to do by hand and how much you can use the readily available free tools to help you.

The way I've described this approach leads naturally on to the next logical step which is to go to full CNC. There are many piecemeal ways to use a DRO but that wasn't intended to be the focus of this thread.

Perhaps I should have called out something else, but MNC seemed to be a sensible title at the time. It wasn't my intention to hijack the term.

[doubletop]

Sept 2, 2018 20:23:07 GMT Roger said:

I suppose it depends on how much work you want to do by hand and how much you can use the readily available free tools to help you.

The way I've described this approach leads naturally on to the next logical step which is to go to full CNC. There are many piecemeal ways to use a DRO but that wasn't intended to be the focus of this thread.

Perhaps I should have called out something else, but MNC seemed to be a sensible title at the time.

Rodger

Some of the approaches you are taking with CAD can be done directly with the DRO's. Your example of a port in a cylinder block is an out of the box function. Work out the starting point from the drawings and then use the line of holes function with a very small step. e.g, precision chain drilling.

Then again as the port will be square to the job you don't even need to do that once you know where to start and end. Drill a hole at the start point, change to an end mill and incrematally move up the line punching down on the quill. However, with DRO's you could have your port at any angle you like and do the same thing. The DRO's will work out the tool path and direct you to the next step. No need to transfer any coords from the G Code so no need to spend time learning CAD and drawing it up.

We've got the opportuinity here for a very useful thread for others, if we just walk them through it.

Pete

[Roger]

Sept 2, 2018 20:36:10 GMT doubletop said:

Sept 2, 2018 20:23:07 GMT Roger said:

I suppose it depends on how much work you want to do by hand and how much you can use the readily available free tools to help you.

The way I've described this approach leads naturally on to the next logical step which is to go to full CNC. There are many piecemeal ways to use a DRO but that wasn't intended to be the focus of this thread.

Perhaps I should have called out something else, but MNC seemed to be a sensible title at the time.

Rodger

Some of the approaches you are taking with CAD can be done directly with the DRO's. Your example of a port in a cylinder block is an out of the box function. Work out the starting point from the drawings and then use the line of holes function with a very small step. e.g, precision chain drilling.

Then again as the port will be square to the job you don't even need to do that once you know where to start and end. Drill a hole at the start point, change to an end mill and incrematally move up the line punching down on the quill. However, with DRO's you could have your port at any angle you like and do the same thing. The DRO's will work out the tool path and direct you to the next step. No need to transfer any coords from the G Code so no need to spend time learning CAD and drawing it up.

We've got the opportuinity here for a very useful thread for others, if we just walk them through it.

Pete

Hi Pete,
I agree, there's much of use here and lots of ways of going about things.

Machining a port or profile using the CAD/CAM method is different from using DRO functions in two respects.

Firstly, the coordinates created by the CAM program initially create an under sized feature. That feature is measured and fed back into the CAM so that it can create new coordinates to bring it to size. You change one figure and get a completely new set out coordinates that reflects that change.

Secondly all of the ports can be defined in one set of operations to do the whole process with just one master reference point. When you measure and correct the size on one port, the corrections are carried across the others.

It's also worth noting that you can change the cutter size and instantly get a new set of coordinated that reflect that change. These are powerful features that take it way beyond what built in DRO function do.

[Deleted]

You've both doing a great job but as this is all very new to me I'd certainly like to start from the beginning. I won't be using CAD, just want to get the best from my planned new DRO

Pete

[simplyloco]

Sept 2, 2018 20:36:10 GMT doubletop said:

Sept 2, 2018 20:23:07 GMT Roger said:

Rodger
SNIP

We've got the opportuniity here for a very useful thread for others, if we just walk them through it.

Pete

Pete
I have to agree with you. I downloaded Fusion 360 today. I am on lesson seven and it is amazing stuff, especially the sharing facilities and version control. I have 'O'level tech drawing, and I taught myself 2D Autocad (V2.7) in the 80's, so I could fancy myself having a go at it. However, this fabulous software is a very large sledge hammer to crack my quite small nuts and I won't be exploring it any further. I'll stick with my (free) DoubleCad.
As you suggest, the built in DRO functions will suffice., but I have to say that whilst the precise positioning facility is rather nice for one offs, for repetitive work I still find myself relying on saddle stops and marked points on the dials, as I prefer to look at the work rather than watch the screen while I try to get the right numbers to appear!
John

[simplyloco]

Titans of CNC

This guy has spent a lot of time and effort promoting American manufacturing. There is a whole series of videos (overblown and typically American) on 'How To' with Fusion 360.
Here is just one example, covering early learning, and I found it quite interesting. At the 10 min. point he creates threads just like that!
John

academy.titansofcnc.com/series/titan-1m/how-to-draw-the-titan-1m-2

[doubletop]

It’s temporarily gone a bit quiet on this thread. Roger and myself are having a bit of side conversation on the best way to approach this topic without confusing the hell out of you all and making it useful wherever you are on the continuum of basic mill, DRO's, CAD, CAM to CNC.

If we get it right there will hopefully be lightbulb moments for some and no doubt some 'suck egg' moments for others.

Pete