Advanced 3D CAM and 3D machining

[Vixen]

Edit Jo: This thread has been extracted from the Mercedes-Benz W165 Grand Prix engine in 1:3 scale as it started to get into detailed (and important) CNC stuff

The work is incredible. This sump part really catches the imagination for what is possible.

estlCAM is also Windows software, but you  say (or at least imply) that you are using estlCAM on Linux. I have searched about and it seems many people have had success using it with Linux Wine emulation. Is that true in your case?


--Tim

Hello Tim,

Sorry if I have mislead you. All my machine tools in the workshop have a dedicated LinuxCNC PC driving them. I maintain an ancient 32 bit Win XP PC in the office to run AutoCAD, DesKAM and EstlCAM and to access this forum

Mike

[tvoght]

Oh, ok.
Nevertheless, if I can get estlCAM to run on Linux (and it's apparently quite possible) I think I'll give it a try for g-code generation since it's quite affordable and the results (your results) are great.
--Tim

[Hugh Currin]

Mike:

Were you able to use a CAM program directly for the Woodruff Key cutter? Or draw special path lines to follow, maybe even hand code those paths? It sounds to me like a hard thing to do, either being real careful with the plunge and entry clearances or hours verifying hand code. Do you have a simulator to verify G-code?

The part looks amazing and way beyond my capabilities. Thanks for posting the build.

[Vixen]

Hello Hugh,

Most, if not all, CAM programs assume the milling cutter to be cylindrical. However, you can still enter the diameter of the Woodruff cutter or slitting saw to create a tool path, which will then need some manual editing. It is essential that you take control of the z movement positions; the vertical moves must re-positioned be well clear of the material. You will have noticed I  hack sawed off a lot of the excess material on the sides of the sump. This gave space for the Woodruff cuter to descend into.

For the tool path, I again used EstleCAM in the peel mode. I set the step over depth of cut to something like 0.5 mm (I cannot remember precisely what I used) to reduce the contact length of the cutting edge of the Woodruff cutter. This is part of the tool path it produced for the top fin. There was plenty of table movement and machining of fresh air for the small amount of material removed. Each fin took about 1 hour to finish. There may well have been a more efficient way to cut the fins but this worked for me.





Mike

[fumopuc]

Hi Mike, very impressive.
I am sure it took some hours of virtual milling before you are feeling safe to press the start button of each tool path at the machine.

So it would be if I would try it.
Very nice result so far.

[Vixen]

Achim and Hugh

I edit the g-code until the pre-view screen or simulation is doing what I think it should do. Then I normally do a trial run on the milling machine with the Z zero set a safe distance above the work. This usually shows if the g-code is about right. Then it's: set the z zero height correctly, Press the Go button and see what happens. I usually slow the feed rate down for the first contact with the enemy. I turn the feed rate back up, as confidence grows.

Mike

[Jasonb]

You could also have done it as a cut following around the edge, set it with multiple roughing passes each of 0.5mm totalling the max thickness to be removed and similar feed to the peel one you used. One for each height with a large lead in radius. The good thing with the simulators is you can try out the various options in the comfort of your study and then once happy go and make swarf rather than have to fiddle about in the workshop.

Something like this assuming the waste corner had been sawn off. Yours would probably rapid to the other side and then rapid across to the front to take the next pass but I just drew the half you showed

[Vixen]

Hello Jason,

You are quite right, there ARE many, many, different ways to machine those fins. Fusion, no doubt, would offer more options than I have available. I chose one method and it worked. Thats good enough for me

My alternative would have been to create a concentric contour tool path by telling a lie to the CAD about the true tool diameter. Start by declaring the cutter has bigger than it actually is, then repeat at several smaller false diameters until you reach the true cutter diameter. Edit all the tool paths into one to produce a combined concentric tool path. That also works well, but can be more time consuming.

You can only use the tools you have available.

Mike

[Hugh Currin]

Mike:

Thanks for the explanation. I'd have started down the path Jason mentioned. But it looks like the fins are a 3D contour rather than just square. It may be difficult to form the 3D surfaces with the scheme Jason suggests. I suspect the contouring leads to the multitude of tool paths you show? I glanced at EstleCAM but didn't see much about their 3D machining. It must be in there though as you've sure figured it out.

I'm using Cambam. I've looked at their 3D machining on the computer but haven't cut a part using it. It seems workable but not robust and has none of the "advanced" adaptive/peel options mentioned. I'll work towards getting Fusion running on a Linux box which would give me better CAD and CAM functionality. Just take a year or so to learn.

Again, marvelous parts and overall engine. Although I'll never be at that level, I'm learning a lot following along.

Thanks.

[Vixen]

Hello Hugh,

EstleCAM is only 2.5D not 3D machining. I tried Cambam, but could not get on with it.

3D machining is way above my pay scale, so I will stick to the 2.5D machining that I know, for now.

However, when you get Fusion to run in Linux, I will be happy to give it a go.

Mike

[Vixen]

Hugh,

Just so that you don't get the wrong idea about how I did the 3D profiling inside the dry sump. The tool paths shown below are just a stack of 2.5D contours added together to make one big file.





Mike

[crueby]

For a non-cnc guy, what is '2.5D'?   

[ddmckee54]

Crueby:

2.5D is where the software assumes that the cutter movment for each pass will be in the X-Y plane, and then allows the Z axis to be moved between passes.  Each of the contour lines in the above picture would represent a horizontal pass of the cutter.  You get a close approximation of the 3D part that will contain small steps.

Don

[crueby]

Crueby:

2.5D is where the software assumes that the cutter movment for each pass will be in the X-Y plane, and then allows the Z axis to be moved between passes.  Each of the contour lines in the above picture would represent a horizontal pass of the cutter.  You get a close approximation of the 3D part that will contain small steps.

Don

Thanks Don!

[Hugh Currin]

I think of 2.5D as horizontal and vertical surfaces only. You're developing 3D profiles which include the Z axis, which I think of as 3D programming. For example the Z-X arc on the right side in this drawing. It could be thought of as 2.5D since you're moving down in Z and finishing that level, then move down Z and repeat the new level. But it's more a waterline tool path, like following contours on a map, to get a 3D shape.

Are you figuring out the tool path at each level and manually combining these into a program? Or is the CAM package figuring out the ball end mill path at each level and giving you back one complete program? The manual process sounds very tedious and time consuming. I know it's possible, George Britnell does similar on a manual mill (not sure how he does it but he gets amazing results).

If you're doing this manually then I think we both need to find a good 3D CAM package. If you're program is doing it for you, then it's only I who needs to find such a package.

Either way great work. Thanks for the help.

Hugh,

Just so that you don't get the wrong idea about how I did the 3D profiling inside the dry sump. The tool paths shown below are just a stack of 2.5D contours added together to make one big file.



Mike

[Jasonb]

I'd say 2D is horizontal and vertical surfaces only. 2.5D is when you increment down and run another horizontal and if that downwards increment means the tool needs to move sideways compared to the previous cut then that is how it copes with slopes doing them like contours on a map. The down side of this is if the shape is curved rather than just a straight angle then the horizontal stepover is less on near vertical surfaces and increases as they become flatter.

3D will follow the slopes and curves better and can adjust each "level" so that the step or scallop between cuts is constant no matter what part of a curve is being cut. Also instead of the the tool doing a horizontal path each time it can be constantly ramping down in effect following a spiral around the shape of the part. When the tool really starts to move about is when you have compound curves such as fillets where one curved surface meets another and then you see all 3 axis moving all over the place at the same time. For all of these you just select the overall shape or surface and the CAM will work out a single path, no need to string them together. Though you would usually do a roughing adaptive cut and then a finish or two selecting the best approach for each aspect of the part.

This is a short video I did at the weekend for someone who had only been using 2 and 2.5D and wanted some curves on some steel parts. Their first attempts produced a program that took 56mins on the simulator. This is the part being done in 7mins. (they had 16 to make) You can see on the adaptive how the 1mm vertical stepdown results in wider stepover as the curves flatten out towards the bottom. I then did a scallop on one side and a parallel finish on the other. Though in the end orientating the work vertically would have given the better surface finish.

<a href="https://www.youtube.com/watch?v=cj7lD1hIJro" target="_blank">http://www.youtube.com/watch?v=cj7lD1hIJro</a>

[fumopuc]

For a non-cnc guy, what is '2.5D'?   

Hi Chris. a lot of wise explanation is given already. I like this forum for that very much.
Your closest example for 2.5 D should be your new toy, the so called "3D" printer.
In reality it is working in 2.5 D only.
Creating the part in x and y by small layers.
What Jason has shown, the "parallel" machining, specially the finishing of the second side of the part, is something what the hobby "3D" printers are not able to do.
But that is what I do understand by 3D machining.

[Jasonb]

I'd actually say the scallop on the front side is far more £d than the parallel on the back.

On the parallel the work "puts on a cut" in the X direction (the 0.5) and cuts using Y & Z (the 2.0D) giving the total 2.5D, if you watch the DRO readout at the end you can see X only moves in steps between cuts.

On the Scallop the tool is constantly moving in all three planes so true 3D.

J

PS Jo thanks for moving things I was actually thinking of PMing Mike and asking if he wanted me to move my earlier reply to a new thread rather than hijack the build.

[john mills]

when i was programming cnc machines i did not have cad cam programs and the computer programs worn't
powfull enough to do much.one of the machines i wrote programs for   ( a mazak v5 ) was only 2.5d
you could only put 2 axis on the one line and not y and z so it was limited to just x and y  but could do x and z so for one job to profile a curved groove the job had to be turned at 90 degrees so i could use and x  g 18 programming using g codes.programing the mazak v10 was able to do 3d as it would do 3 axis at once so i programmed 3d shapes but used subroutine and repeat lines a number of times to produce shapes .often with a
63mmdia facing cutter manually worked out the figures and tool radius compensation to produce the right shape.
mostly machining hot tool steals or some times   high tensile  steels .the cad cam  program that came latter
was not able to sort out the 2 axis on one line for the mazak v5 but i was no longer needed and was retrenched
they would have found out when i was gone.they did not want to know when i told them i had just continued until i left.they would have found out when some one else tried  .the people left  had done little programming and would have had a lot of learning to do  .the cad and the cam programs you have now seam to be able to do these ships on your machines.as i programmed the muzak v 10 the last row of cuts on jasonb video shapes could have been done with the lines to produce the shape an incremental shift  then repeat the number of times required 
John     

[Vixen]

This is getting a bit mixed up. Let me try to clarify things.

I do all my CAD work in 2D, plan view, side view, front view etc. I do not do 3D drawings

My two CAM programs DesCAM (no longer on sale) and EstleCAM are also 2D/2.5D, neither of these programs can do 3D CAM

I create a pseudo 3D surface from a large stack of 2D contours at different heights.(like the contours on a map or the steps on a 3D printer) Each layer (contour) is laboriously created in the 2D drawing package, then made into g-code by the 2D CAM software. This is crude stuff, very slow and time consuming but it does make an interesting intellectual challenge for me. The tool path I showed earlier took several days to prepare, but that was OK by me while I was isolating and confined to barracks. I was not going anywhere.

True 3D modeling and 3D CAM requires much more advanced software and processing power than I have available.  3D CADCAM is intended for the industrial setting. Solidworks, Dasault, AutoDesk are some of the big players and they all require thousands of dollers, pounds or euros each year for the privilege of using there products. All the processing is done their end over the net, the user only has a terminal. Everything is done of the internet, so you need a good reliable connection and bandwidth

However AutoDesk have taken the decision to release some of the Fusion 360 CAD CAM free for the use of students and hobbyists. They see this as an investment for the future, as they expect many of the students to eventually become paying users.

I do not know of anything useful between my crude 2.5D CAD CAM and the high end 3D CAD CAM. That would be a very useful area to explore.

If I were to buy a new hi-spec PC, If I were to go over to Win10 along with all the problems associated with Microsoft control of Win10; I could download Fusion 360 and eventually learn to become a Fusion 360 user like Jason. I cannot see that happening in the near future

Mike

[tangler]

Guys,

My take on 2.5D is slightly different.  The point being that the CAM program takes it's input from a 2D drawing which controls the X and Y movements but the Z movement is a single depth specified by the user.  This system still gives a fair amount of versatility.  Take the example of a simple circle.  The program has been told the diameter of the tool being used.  The options are then to cut around the outside of the circle or the inside of the circle or for the centre line of the cutter to follow the circle.  Additionaly, the program can be instructed to clear inside the circle or outside the circle and can do this with control over the depth of cut for each pass.  The program can follow any continuous single line according to the parameters mentioned above.  Anyhow, that's how the cam system that came with my Denford mill worked.

Cheers,
Rod

[Jasonb]

So Mike, coming back to the "peeling" that got us started do you produce a drawing for the pocket at 6mm deep and then let your CAM workout the path it will take to peel that away. Then do it again for 12mm deep and so on finally combining them all into one long g-code?

If so then that is as you say a long job and also leaves 6mm steps at the edge. With a more upmarket CAM such as F360 all the user has to do is click on the geometry which in this instance could be anywhere along the inner edge of the bolting flange and then just specify a max depth of cut, stepover, feedrate and also a minimum stepdown. The CAM will then work out where the boundry is for each 6mm layer if 6mm is set for max DOC and also once everything has been removed at that level go around the sides again stepping the edge to say 1mm increments leaving less to come off with the finishing passes. It will then do the same again for each multiple of 6mm until the bottom is reached. Note it's usual to specify an amount of stock to be left such as 0.5mm radial and 0.5mm axial which will be removed by the finish strategy.

So much less manual working out involved and it also knows what the roughing passes have left so only does the finish passes to remove the remaining material.

[kvom]

While many 2.5D tool paths just repeat at increasing values of Z, there are some that have coordinated Z motion.  The most common of these are ramped profiles where each G1 command has 3 coordinate values.  There are also helical moves for machining holes and milling threads.

I have been a CamBam user for over a decade, but have done only a couple of 3D toolpaths.  In the past I would take paper plans and draw them in CAD to produce DXF files.  Since I now get SolidWorks free as a veteran, I'll model parts there in 3D, and then export to DXF.  My last two builds I received the "plans" as SW models for all the parts, thus saving a lot of work.

Once I load a DXF file into CamBam, I can manipulate it as needed before applying various operations to selected lines within the drawing.

For the type of pocketing Mike used, CB has an operation called Trochoidal Pocket.  Trochoidal is just a technical term that means the tool's angle of contact with the work is kept constant.  Constant angle means feedrate can be constant as well.  The toolpath for a pocket starts with a straight plunge to target depth followed by an outward spiral.  The position of the spiral is calculated to maximize the size of the spiral within the pocket shape.  The rest of the pocket is completed by successive arcs.  There is an option to machine each alternate arc in reverse direction, but I prefer to just have the tool return rapidly to the next arc allowing any chips to clear the tool.

After this operation, the sides of the pocket will have some scalloping that I remove with a subsequent profile operation.  I specify a roughing clearance of a few thou on the pocketing.

CamBam has a trochoidal profile op as well, and I have used this to machine slots using a tool whose diameter is smaller than the slot.  The advantage in aluminum is that chip welding is eliminated.  I can also cut the slot at full depth.

[Hugh Currin]

Mike: My hat is off to you for the skill and patience to generate tool paths as you do. You're results speak for themselves. If I tried this I'd be tracking down errors for the foreseeable future. Nice job.

kvom: I think I'm about where you are. I use VariCAD to generate 2D *.DXF files and import these to CamBam. I've poked at the 3D features in CamBam but not cut parts with them. I've found I can import 3D *.STL files into CamBam. My older version of CamBam doesn't have the trochoidal generator you mention, but I see it's available as a plug-in. I'll have to get that or upgrade.

I'm trying to get Fusion 360 going for their milling and lathe CAM. Also, the parametric modeling would be helpful in design (once it's learned). I need to pick a project with some 3D (far simpler than Mike's) that would force me to do some 3D milling. But way to many projects already.

Thanks.

[Vixen]

Hello Hugh

Thanks you for that comment. It is always nicer when people appreciate how much effort you have taken, much nicer than receiving flak for not using the latest and greatest.

Incidentally, the 'peel' pocketing of EstleCAM is trochoidal milling. 'Peel' was a shorter word to put on the function select button. You can trochoidal mill a pocket or trochoidal mill an inside or outside profile. There are also options to rectangular milling or to raster mill out pockets. I actually like the term 'Peel' to me it conjures up images of a pencil sharpener peeling off a thin shave of wood.

Mike

[fumopuc]

I'd actually say the scallop on the front side is far more £d than the parallel on the back.

On the parallel the work "puts on a cut" in the X direction (the 0.5) and cuts using Y & Z (the 2.0D) giving the total 2.5D, if you watch the DRO readout at the end you can see X only moves in steps between cuts.

On the Scallop the tool is constantly moving in all three planes so true 3D.

J

PS Jo thanks for moving things I was actually thinking of PMing Mike and asking if he wanted me to move my earlier reply to a new thread rather than hijack the build.

Hi Jason, you are right. I have been focused so much to the continuous up and down movement of the Z axis that I missed the only step by step movement of the x axis here.
As you mentioned already, the scallop movement at the other side is a much better example for 3D machining/movement. 

[Jasonb]

Maybe I was confused by the title of "Advanced 3D CAM..............." and thought that it was a place to discuss 3D CAM

Hugh it would certainly be worth trying to get F360 to work on your machine, as you say it's not just it's CAM capabilities but the whole design aspect and having all these integrated into one place so you can easily jump back and forth from one thing to another. It's one feature I miss by using Alibre for my drawings and F360 for the CAM as if there is a major change I want to make to a part I Have to do it in alibre and import a new STL file and start the CAM again, with it all under one Make you can alter a feature and when you click back on Manufacture ( the CAM part) the cutting paths will update with a click of the mouse. I do use Fusion to make small changes and infact there are some things it handles better than Alibre.

It's also possible to use Alibre offline so you can do your CAM when you are traveling about with poor or expensive connection options. Not sure what the system requirements would be on a Linux machine but I don't use anything particularly advances on my Windows PC and only get the odd time it slows F360 down a bit.

Achim happy to clear things up and good to know some take my comments constructively in the way they are meant.

[Vixen]

Maybe I was confused by the title of "Advanced 3D CAM..............." and thought that it was a place to discuss 3D CAM

Jason, your considered contributions will always be welcome. You have more experience with Fusion 360 than any of us. Hopefully the new topic will enable all of us to advance our knowledge of whats available and what it can or cannot do.

Mike

[Vixen]

Mike:
Back in Post #338 you showed a screen shot of the dry sump that showed the depth of cut for each layer.  How did you generate those lines?  I've got my suspicions, but "Enquiring minds want to know".
Don

Don, Jason,

It's funny the way things change with time. I have been building engines, tanks and a lot more in my CNC workshop for nearly 25 years. During that time, I have often taken flack from other model engineers, who say what I am doing is not 'real' model engineering. That's because I am not using the traditional Myford lathe or whatever. Besides CNC is realy cheating; it's too easy, there's no skill, there's nothing to it. You press the button and out pops a completed engine.

Now suddenly, I'm receiving incoming from a totally different direction. I'm now being  told:  "Holy Moly" your doing it all wrong. That's definitely a long winded way to do it and how much BS you're willing to put up with? What you should be doing is pressing a button in Fusion 360. The 3D CAD/CAM will work it all out for you and do in minutes what can take you several days to do. The same model engineers, I mentioned earlier, may now rightly say "it's too easy, there's nothing to it. You press the button on Fusion and out pops a completed engine." Where is the skill in pressing that button?

As I have said before: I have 2D CAD and some 2D/2.5D CAM. I have no 3D stuff. I come from an old school which tought me "use what I have available and make what I dont have."  I am happy to apply that philosophy to my engine building. It may be slow, it may be long winded but it gives me immense pleasure and the results speak for themselves.

As to how I generate those lines? I use 2D CAD. You know: plan view, side view, end view. and the occasional cross section. For my pseudo 3D work I simple create (by old fashioned drafting) a number of cross sections at about 0.25 mm (10 thou) spacing and even closer spacing where rate of curvature is greater. These cross section contours are transferred as individual DFX files to my 2.5 D CAM which does the tool path G-code conversion.  I combine all the G-code(s) into one big file. OK it's slow, it's long winded, it's old fashioned, it's probably the way Noah built his Arc. But it works well enough for me. I'm in no rush,  I'm not going anywhere for a while yet.

Dont get me wrong, I have nothing against 3D CAD CAM. I would dearly like to use it if I get the opportunity. Maybe someone would sponsor me and provide a nice new computer, Maybe someone will assure me that MS will not mess about with Win 10 while I am using it. And most importantly; Maybe someone will assure me that Autodesk will not suddenly change 'free' Fusion 360 into FEE Fusion, when they think they have hooked enough users.


Now lets cool thing down and enjoy our Model Engine Making

Cheers   

Mike

[Admiral_dk]

I'm sorry if it sounded as I has anything against your methods Mike - I just know how many errors that usually creeps in the .nc (G-Code) files when I edit them manually -> I'm very impressed with your results.

Per

[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