Advanced 3D CAM and 3D machining

[Jasonb]

Well as I said I'm sorry if you see it that way.

I have said it here and on other forums that I was put off CNC by the thought of having to learn G-code and watching guys on the SMEE stand take ages to do something that could have been done with a manual machine far easier and quicker so much so that I turned down the offer of a CNC machine some years back.

Wind forward to a couple of years ago and another offer came up which after some thought I accepted which arrived with a 2" thick book about CNC programming However I had read mention of the likes of Fusion and gave it a go and found it easy to get on with and it produced tool paths from the 3D drawings I was already happy producing. That is why it thought others may like to know how it makes getting the most out of a machine less of a daunting task and will hopefully encourage other readers and participants in the thread to go over to the dark side and try CNC.

I think getting an understanding of how you actually produce the code for what you do has left us more in oar at what you do with what you have available.

[JimG]

I've just picked up on this thread.  I've got an eleven year old Seig KX1 recently upgraded to use an ESS controller to get away from the original parallel port interface.   When I first got it I intended to use it for full 3D cutting and purchased a copy of Vectric Cut3D to do the CAM work.   But results of 3D machining were not all that good and I eventually found out the hard way about the Seig "nod" whereby the head effectively pivots around the slideways of the head when the Z direction is changed.   I tried adjustments and counterweights with no real improvement.

So I now do the same as Mike when I do need 3D machining and write my own Gcode to do waterline cutting of parts with the Z decrementing in the same direction for each line of cutting.    For example for a part with a semicircular section I start at the top and go down one side then restart at the top and go down the other side.   

For example, one of the jobs I do is 2.5D cutting of 1:32 scale model railway coach sides.  The prototypes are of the Victorian/Edwardian era with panelling,  and Vectric Cut2D handles the majority of the cutting in 2.5D.  But a feature of these coaches is the shaped bolection mouldings around the quarterlight windows and I do this in 3D with my hand coded Gcode.   I use 2D CAD to work out the X, Y and Z values then make a subroutine in Gcode with generates the rectangular shape of the window with curved corners and accepts variable inputs for the layers of waterlines and the position of the bolection.   I dry run in Mach3 to check that there are no problems.

I also use Fusion 360 for my 3D printing work and I have followed Jason's thread in the Model Engineer forum when using it for 3d CAM on his KX3.  But I haven't ventured down that road since I suspect I'll get results which are less than perfect.

Jim.

[Vixen]

Hello Jim,

Thanks for your input, it's good to know I am not the only one out of step.

A number of the so called 2.5D cam programs also offer some 3D capability. Both my DesKAM and EstleCAM can produce 3D toolpaths from STL files. EstleCAM offers both raster and waterline tool paths and seems the more capable.
Have a look at this video.

<a href="https://www.youtube.com/watch?v=xw0ZFf75lAM" target="_blank">http://www.youtube.com/watch?v=xw0ZFf75lAM</a>


I have not yet fully explored the EstleCAM capabilities. However I have tried raster mode machining using other software. The Raster mode is best used for low relief (bass relief) objects as shown below.  I needed to use a very low feedrate because I only had a 2,000RPM spindle at the time and was using a 1.5 mm ball  nose cutter. The X, Y movements were no problem but the Z-Axis was clearly suffering. The 8.0 Kg head and spindle were going up and down like a woodpecker. The waterline mode will be much gentler of the Z-axis and may be useful for deeper objects. I have yet to give it a try.

This sweet little cameo measures 30 mm x 43 mm and took several hours to machine, due to the low spindle speed and the abuse being given to the Z-axis. It was raster machined in both the vertical and horizontal directions. The original must have been hand engraved by a true craftsman.




All I need to do now is to learn how to convert some of my 2D drawings into STL files.

Mike

[Jasonb]

Jim. F360 has various finishing options, something like RAMP will work out it's way around a shape while constantly lowering the tool not even stopping and starting at each height and would actually be a better option for something like the moulding that you describe than one where the tool is going up and down all the time, infact I would think even scallop would tend to mostly run along the moulding rather than up and down. You choose the best option for the job or feature.

Or you can use a simple contour which will produce a similar path to what you and Mike describe doing manually by working out the path it needs to follow at any given height increments and all the time moving the head down for the next increment. You can split any curved surface up into a number of sections and use different vertical steps as the curve flattens out or becomes steeper. You do need to decide on these sections Manually unless paying for the "Steep and Shallow" option which even works that bit out for you.

[mikemill]

I use a fourth axis (horizontal rotary table) to create a 2.5D way of machining, whereby you draw parts in 2D and cut, then rotate to whatever deg required and cut the same shape or different shape. I use this way to make forked ends of eccentric rods in one go.
Those who pour scorn on CNC machining do from a lack of experience with these wonderful tools, as to skill try making a part using CNC with no knowledge of the process, then say no skill!!!
I have been a model engineer for over 50 years and built many engines of all types before acquiring a CNC mill. In the last ten years I have had more fun using the CNC mill than I can say.
I have just completed this G3 GWR Armstrong Goods Engine, with the exception of the electric motor the model is entirely built using the CNC mill and manual lathe, the number plate was engraved with a 0.030in chisel point tool on the mill.
The engine has fully working inside motion R/C and sound with batteries and electronics housed in the tender.

Mike

[JimG]

Mike,

A number of the so called 2.5D cam programs also offer some 3D capability. Both my DesKAM and EstleCAM can produce 3D toolpaths from STL files. EstleCAM offers both raster and waterline tool paths and seems the more capable.

I have not yet fully explored the EstleCAM capabilities. However I have tried raster mode machining using other software. The Raster mode is best used for low relief (bass relief) objects as shown below.  I needed to use a very low feedrate because I only had a 2,000RPM spindle at the time and was using a 1.5 mm ball  nose cutter. The X, Y movements were no problem but the Z-Axis was clearly suffering. The 8.0 Kg head and spindle were going up and down like a woodpecker. The waterline mode will be much gentler of the Z-axis and may be useful for deeper objects. I have yet to give it a try.

I had a look at the video and I think EstleCAM does much the same as Cut3D.  It's been a few years since I used Cut3D so the memory is a bit hazy and I think it was installed on an older PC which is no longer in service so I can't run it to see.     I do remember at the time I was having the problems that there was a CAM application which provided waterline cutting but it was a bit pricey for me at the time.  I also remember finding out the problems with raster cutting and the Z axis having to bounce up and down at high rates with deep subjects with near vertical sides. 

I'll have a closer look at the CAM provision in Fusion 360 as suggested by Jason to see if I can get something ressembling waterline tool paths to cope with my nodding Z axis.

Jim.

[Vixen]

I have been a model engineer for over 50 years and built many engines of all types before acquiring a CNC mill. In the last ten years I have had more fun using the CNC mill than I can say.
Mike

Mike,

Your magnificent loco speaks volumes about your CNC skills. Beautifully machined and beautifully finished and painted.

No.....CNC does not make it easy, but it sure does make highly detailed model engineering, like that,  possible.

Mike

[JimG]

Jason,

Jim. F360 has various finishing options, something like RAMP will work out it's way around a shape while constantly lowering the tool not even stopping and starting at each height and would actually be a better option for something like the moulding that you describe than one where the tool is going up and down all the time, infact I would think even scallop would tend to mostly run along the moulding rather than up and down. You choose the best option for the job or feature.

Or you can use a simple contour which will produce a similar path to what you and Mike describe doing manually by working out the path it needs to follow at any given height increments and all the time moving the head down for the next increment. You can split any curved surface up into a number of sections and use different vertical steps as the curve flattens out or becomes steeper. You do need to decide on these sections Manually unless paying for the "Steep and Shallow" option which even works that bit out for you.

I'll have a dig around in F360 to see if there's something that will suit my KX1.  It might take a while since it has taken a bit of time for me to prise myself out of years of 2D drafting experience to get my head round F360 for my 3D printing work.     I'm up to my eyes in another project at the moment but I'll have a look at some of the Youtube videos on F360 and CAM to see if I can pick up any hints.

Jim.

[Jasonb]

That loco certainly look very nice particularly the satin almost matt finish to the paint and even the metal

If you can post an image of the bolection moulding or actually the way it goes around the door as I know what bolection moulding is like I'll have a play and post something.

I do still get a bit of a step where it changes from up to down but have reduced it a lot from when I first stated to use the machine, mostly buy easing the gib strip which was making the head stick, it does also seem to be affected by the material as on iron and steel it seems greater than on ali or wood so may also be a bit of the material pushing back against the tool.

I did this piston top yesterday, as it was fairly flay and the curved top only runs in one direction I used a parallel path with 0.2mm horizontal spacing which gave about 120 passes, it worked out each vertical move by itself and all those verticals were outside the area of the top. The actual 3D modelling way just two 2D sketches one the 24mm circle that was extruded for 27mm and the second a side profile of the top shape that was removed right across the previously drawn cylinder. CAM was one roughing operation where it worked out the 0.5mm heights itself as stopped the edge of the tool to leave 0.3mm. Finishing pass was as mentioned above

[kvom]

One use of 4th axis in CamBAM (or other 2.5/3D CAD programs) involves wrapping 2.5D code around round stock.  For example, assume axis of rotation is X.  You generate the g-code as normal, and then modify it via a separate program.  X coords remain unchanged, and Y coords are changed to A coords with the distance converted to degrees according to the specified stock diameter.  G2 and G3 can't be used, so arcs must be generated as a series of small linear moves, and option provided by the CAM software.

Of course, simpler uses of the 4th axis can be coded by hand.  If you are machining the cylinder decks of a rotary engine, then regular 2.5D work on a deck can be used, with the work turned 40 degrees (9 cylinders) by manual command.

[kvom]

One option for this type of work is a height map.  With A b&w photo as input, divide it into pixels whose values depend on the level of grey and black, the result being a 3D surface.  CamBam has a plugin for doing this.  There are possibly other programs that do the same.

[ddmckee54]

Mike:

I'm sorry if that was the way you interpreted what I said, because in no way was that what I meant.  My comments were in no way meant to imply that you were doing anything "wrong".  Quite the contrary, I am amazed and impressed with what you have been able to do with what you've got.  Those are the software packages you've got, you are obviously very familiar with them, and more importantly - you're happy with them.  If you're happy with something there is no good reason to change it, especially when you can get the results that you have demonstrated.

If all those contour lines were generated using 2D Cad, I'm even more impressed.  Having had to do similar things in the past, I know how much work it is to do that.  (Especially to get it right, as you obviously did.)

Again, sorry for the miss-understanding,
Don