3D design to CNC mill design flow

Advert

New Replies

Report Bug

Help/FAQs

3D design to CNC mill design flow

This topic has 28 replies, 9 voices, and was last updated 17 December 2016 at 23:47 by Roger Head.

Viewing 25 posts - 1 through 25 (of 29 total)

1 2 →

Author

Posts
13 December 2016 at 14:47 #15131
Roger Head
Participant
@rogerhead16992
How does it all happen?
Advert

13 December 2016 at 14:47 #271573
Roger Head
Participant
@rogerhead16992
This is one of those times when I don't know enough about a subject to even ask coherent questions. This is all pie-in-the-sky stuff, it'll be a fair way down the track before anything happens – if ever. But here goes with just a couple of simple (ha-ha) questions, hoping any answers will either point me to somewhere/somebook/something where I can start to learn in a cohesive way, or will nudge me in the right direction for asking further questions.

1. I've never used 3D CAD software. I've never had any association with CNC
machining. I'm an EE (retired), I've designed, built, and written the code for lots of scientific equipment that required servo/stepper controls and so forth, so the general mechanics of CNC machines hold no fundamental mysteries for me. But the control was by native code in embedded micros, so while I'm aware of G-code, I've never given it more than a very cursory glance.

2. The disconnect in my knowledge is the path from a 3D CAD image to (presumably) an input file for the CNC controller (MACH3 ?). This doesn't seem conceptually difficult for a 3D object containing only orthogonal flat surfaces i.e. pretty simple X/Y/Z stuff. But when the object contains surfaces consisting of compound curves then the machine will (obviously?) require additional axes (rotation about X, Y, and Z). Are there standard assignments that associate drawing rotational axes with machine rotational axes? Hmmm, thinking about that further, it probably shouldn't matter what axes the image is drawn around. Provided the CNC machine itself has sufficient axes, it should be possible to transform the image coordinate system to suit the machine (true or not?). Although it would probably be best if the design coordinates and the envisaged workholding method were designed to map directly to the target machine (true or not?).

3. The end result of this thought exercise is to determine what hardware (CNC mill) and software would be required to design and fabricate a single blade of an axial compressor. The blade would have a cambered airfoil section, with twist from root to tip, tapered thickness, and various planforms – hence all the compound curve questions. I think 4 axes would be sufficient (although possibly not with the 4th axis as the 'usual' (?) rotation about the machine spindle axis), but in any case I need to understand how the CAD design becomes suitable G-code for a given machine. Is the operation intended to be automatic, or does it need further directing by the designer?

As I said at the beginning, I barely know what it is that I don't know.

Edited By Roger Head on 13/12/2016 14:49:48

Edited By Roger Head on 13/12/2016 14:51:58
13 December 2016 at 15:24 #271585
David Jupp
Participant
@davidjupp51506
A few comments – for complex geometry, you really need CAM software to help generate the G-code. No this isn't automatic, you have to do some of the work by splitting the job into operations, and then telling the software which parts of the design each machining operation applies to.

For a single blade I agree that 4 axis capability should be enough – but it must be 4-axis continuous machining not just 4 axis indexed. Some CAM packages skirt around this distinction in the descriptions.

You should be able to find demo videos for this kind of thing on the web sites of various CAM packages. If they don't have a video showing something like this, then assume the software can't do it unless you see hard evidence that it can.

And yes, you have to tell the CAM package about the CNC machine that will be used, that isn't generally too difficult.
14 December 2016 at 00:15 #271672
Roger Head
Participant
@rogerhead16992
Thanks David, a little enlightenment plus a useful nitpick ("it must be 4-axis continuous machining not just 4 axis indexed. Some CAM packages skirt around this distinction in the descriptions). I had assumed that if something (hardware, software, …) was described as having 'N' axes, then all could be active simultaneously. A valuable point.

Thinking about milling compound surfaces, it seems that (apart from the roughing out from an initial lump of material) it eventually becomes a case of milling 'lines', either with say, a plain endmill, or if it is a concave surface, a ball-endmill. Especially in that latter case, and accepting the variability between materials, what sort of final surface finish is achievable? Something similar to that obtained with a normal endmill on a flat plane, or is some form of finishing process typically required?
14 December 2016 at 00:56 #271674
David Colwill
Participant
@davidcolwill19261
A good starting point would be Fusion 360. This contains the drawing package and Cam module in one. It has post processors for most of the hobby control systems (mach 3 and EMC being the two main ones). There are plenty of youtube videos on how it all works. NYCCNC is a good channel to see what it can do.

The good thing about it is it is free if you turn over less than $100,000 per year.

David
14 December 2016 at 07:43 #271687
David Jupp
Participant
@davidjupp51506
Roger, I'm not an expert on this (have simply had to learn enough to be able to demo one of the available packages) – CAM software typically allows you to define a maximum allowable deviation from the surface of the CAD model. The toolpaths will be worked out to achieve this. Choice of tool size and step-over is typically down to the operator, for some geometries these will influence best achievable accuracy and finish. Like many things, there will be a compromise between machining time and achievable finish. There are other subtleties to handle (like deviation of tool from nominal size (tool wear)

Others may be able to offer better insights on achievable surface finish, and likely necessity to follow up with a polishing operation. It occurs to me that you should pay particular attention to the rigidity of the 4th axis if wanting to achieve good finish.
14 December 2016 at 08:09 #271691
Bob Rodgerson
Participant
@bobrodgerson97362
Fusion 360 is a good starting point for 3 axis work but doesn't at the moment go to 4th axis. I believe 4th axis will be available soon. I use Sprut Cam to generate the G-code, leaving only the simple stuff that my feeble brain can cope with to manual generation of G-code.

There are other CAM packages that are free but I have not tried any.. A book worth looking up is the CNC Handbook by Peter Smid, it is comprehensive however it is a fairly expensive tome.
14 December 2016 at 09:58 #271697
David Colwill
Participant
@davidcolwill19261
I thought the 4th and 5th axis was implemented in the last update. I haven't tried it though. It maybe that you need fusion ultimate to access the full features but I'm pretty sure that there is some functionality for the non paying users.

David
14 December 2016 at 10:58 #271705
Bowber
Participant
@bowber
A little more general info, apologies if I cover something you already know

For most CNC jobs you may find 2.5D is the best fit, this is just the tool moving on one layer at a time and a lot of CNC machining is just that with 2D CAD drawings of the profiles being used.

Items like the fan blade would need to be drawn in 3D CAD but I'm not sure continuous 4th axis machining would be essential and stepped 4th axis may work fine, however you may get smoother machining from continuous 4th axis.

You can hand code for some 2.5D jobs but importing a 2D CAD drawing of the profiles into a CAM program is usually faster, programs like Fusion 360 has both CAD and CAM in the same program (you also mainly work in 3D) so no import is needed and they also have the advantage of updating the CAM if you alter the part

3D CNC gets more complicated and you generally always need a CAM program to create the toolpath. Most CAM in the hobby range will output these toolpaths as very small linear moves so a large file could have millions of lines of code. Some of the commercial CAM are now taking an allowable error and using that to create a lot of small curves.

Some CAM programs to look into:

Sheetcam – 2.5D CAM, aimed at Hobby use mainly
CAMBAM – 2.5D CAM but some drawing capability, again mainly hobby use but it's a while since I looked at it.
Vectric do a range of programs that are very good and usually are CAD/CAM in the same program.
Meshcam – 3D CAM, indexed 4th axis and mainly linear moves but I think the developer is moving towards including curves.
Fusion 360 – 2.5D & 3D CAD/CAM, very modern comprehensive program but a bit of a learning curve.

These are programs I've used and there are a lot of other programs to try but out of these I've mainly use sheetcam with some use of Meshcam for a few indexed 3D items, I now use Vectric Vcarve for most of my 2.5D cutting and I'm getting used to Fusion 360 and have used its output on my son's 3D printer.

I'm only a hobby user so my experience is limited to machining my own hobby parts so I'm open to correction but I hope I've provided a bit more information on the process.

Steve
14 December 2016 at 10:58 #271706
Muzzer
Participant
@muzzer
It does 4th axis as "wrapped path" currently and I think the true ("simultaneous&quot 4 and 5-axis capability is due very shortly. The good news is that for the hobby and small business user, the "ultimate" version with all the CAM extras is free, so by the time you bottom out how it all works, the true "simultaneous" 4 and 5 axis CAM should be ready for you.

There's loads of good tutorials by the Fusion 360 team (and others), an active forum and a product roadmap.

As David Colwill suggests, John Saunders (NYC CNC) has also done a load of videos showing how it all works in a real workshop. Like a lot of things, it's worth spending time to learn about it before diving in an expecting quick results.

Murray
14 December 2016 at 12:00 #271718
David Colwill
Participant
@davidcolwill19261
Posted by Muzzer on 14/12/2016 10:58:27:

It does 4th axis as "wrapped path" currently and I think the true ("simultaneous" 4 and 5-axis capability is due very shortly. The good news is that for the hobby and small business user, the "ultimate" version with all the CAM extras is free, so by the time you bottom out how it all works, the true "simultaneous" 4 and 5 axis CAM should be ready for you.

Murray

Thanks Murray

I hadn't realised that the free version was "ultimate"

Although I have had fusion I haven't really used it much. I've spent the last week tweaking my little mill (Triac ATC) and am getting the hang of the cam side of Fusion. I have run several programs now without any problems.The last job on the list is setting up the 4th axis and getting Fusion to work it..

There are a huge number of drawing / CAM options out there but I haven't seen anything else with this kind of functionality that is basically free.

One thing I have started doing which has been a great help is to create a text document that explains step by step how to do various operations eg setting tool offsets in the ATC, setting the tool table in fusion and basic workflow on running a program. I find that sometimes I don't get much time in the workshop and when coming back to these things after some time I can spend a lot of time trying to remember what I did. I have written off more than 1 expensive cutter by making a stupid mistake usually caused by forgetting to do something.

David
14 December 2016 at 12:19 #271722
Roger Head
Participant
@rogerhead16992
Thanks everyone, you've been very helpful. I've spent quite a few hours with google today, basically discovering how rare continuous 4th axis capability is. It came as quite a surprise. I imagine it is available in high-end products like Solidworks etc, but I haven't even bothered to look at their sites because I've heard what their prices are like – my pension wouldn't cover it. In that same context, Sprut CAM appear very coy with their prices, and only offer a 30-day trial, so I get the feeling that they are out of reach as well.

As several of you have pointed out, Fusion 360 sounds almost too good to be true (good product + FREE! ). I had a look at their RoadMap, which reads well, and will be even better if it becomes true. I watched one of the John Saunders videos right through. Naturally it didn't mean much to me, but I definitely liked the presentation format, and his speaking style. It looks like it would be a great resource if they are all similar.

I read through the Fusion 360 thread (http://www.model-engineer.co.uk/forums/postings.asp?th=108196&p=4) and on page 4 I see several posts by Neil Lickfold illustrating some early adventures cutting model aircraft propeller blades on his (presumably 3D) router. That was early this year, so definitely before any 4th-axis release from Autodesk. Conceptually, it's the kind of thing I am thinking about, and that has pretty much decided me on Fusion 360. It will mean using my W7-64 boot, instead of XP. Does anyone know if MS have given up trying to automatically upgrade you when they see W7 updates being loaded? And how I can stop it if it's still happening?

In my google travels I came across a technique called “Sturz Milling”, see half-way down the page at

http://blog.cnccookbook.com/2013/04/08/cnc-4th-axis-introduction/

I can see the intended benefit, but it looks like another complication for the code generator. Is this a commonly available method?

Thanks again,

Roger
14 December 2016 at 13:11 #271729
Anonymous
Posted by Roger Head on 14/12/2016 12:19:40:

In my google travels I came across a technique called “Sturz Milling”, see half-way down the page at

http://blog.cnccookbook.com/2013/04/08/cnc-4th-axis-introduction/

I can see the intended benefit, but it looks like another complication for the code generator. Is this a commonly available method?

Not in my experience. My medium price CAM software (VisualMill) doesn't explicitly offer it; and is, in my opinion, rather weak on 4th axis toolpaths anyway.

If you're using stepover with a ballnose mill and the surface is not far off the axis of the tool, then by default the side of the cutter is working rather than the end. But that is more by accident than design. To make full use of Sturz style milling I suspect you will need a fairly high end CAM program and/or a 5-axis mill. Or write the G-code by hand.

Andrew
14 December 2016 at 14:51 #271743
Raymond Anderson
Participant
@raymondanderson34407
This CAM stuff is beyond me, and I take me hat off to those who can use it. Having seen Siemens NX 5 axis in use i'm just left shaking me head. So all kudos to those who can use it. [ any Cam software ]
14 December 2016 at 15:56 #271763
Muzzer
Participant
@muzzer
Roger

The price of Sprutcam varies according to the features you want. When I asked for pricing in June 2015, I was told that hobby users get it at half price but they only get one (non-editable) post processor. And for true 3D milling (as opposed to 2.5D milling), you need the "3XMill" version which retails at £1700+vat. So for hobby use you can look at coughing up just over £1k. Once I was able to stand up again, I rapidly forgot about Sprutcam and the more I found out about Fusion 360, the better things got.

The add-ons for the likes of Solidworks come in at full price too. If you are lucky enough to have a copy of SW, you can install the free 2.5D version of HSMworks (bizarrely it's owned by Autodesk) but this lacks all the clever adaptive algorithms that account for so much of the progress in tool paths in the last decade. And for reference, Onshape's 3rd party CAM add-ins are charged at professional rates.

The CAM that is included (for free) in Fusion 360 is basically the full, 3D professional HSMworks CAM. That was relatively simple for Autodesk to do given that they own both products – but also a radical step to allow free use for small users. Onshape, Solidworks and the other mid-range CAD developers must be seriously pigged off by that.

Fusion 360 is aimed at the professional market. Most users will end up paying – and probably quite willingly, given the eye-watering cost of purchasing and "supporting" rival products like Solidworks. Interesting times!

Murray
14 December 2016 at 16:09 #271767
John Haine
Participant
@johnhaine32865
Posted by Roger Head on 14/12/2016 12:19:40: Does anyone know if MS have given up trying to automatically upgrade you when they see W7 updates being loaded? And how I can stop it if it's still happening?

MS now charge for the Win10 upgrade so I think the answer is "no". And if you have Win 7 (I do and like it), you can download a free utility called GWX that stops them trying anyway.

I know someone who makes small gas turbines and makes his compressor fans using CNC, I'll ask him what he uses.
14 December 2016 at 16:20 #271770
Anonymous
Posted by Muzzer on 14/12/2016 15:56:47:

Fusion 360 is aimed at the professional market. Most users will end up paying – and probably quite willingly, given the eye-watering cost of purchasing and "supporting" rival products like Solidworks. Interesting times!

And don't even think of asking about Mastercam……….

Andrew
14 December 2016 at 16:40 #271780
John Haine
Participant
@johnhaine32865
Roger, I have sent you a PM.
15 December 2016 at 01:31 #271923
Roger Head
Participant
@rogerhead16992
Having decided on Fusion 360, I will proceed to learn how to create component designs, and then (using the inbuilt CAM capability), create output files. At that point, is there any benefit in having, say, MACH3 without any mill attached? Will it usefully perform any sanity checks on the input file?

Related to that, is there any software that accepts the CAM file and re-creates a virtual component (on the screen)?

Roger
15 December 2016 at 07:49 #271938
David Jupp
Participant
@davidjupp51506
I don't know specifically about F360, but many CAM packages include cut material simulation which starts with the stock material on screen and shows it being machined to finished item.

There are also simple software tools which will plot the toolpath (e.g. NCPlot, or indeed the screens within Mach3). Not quite the same as showing the material, but may be useful nonetheless.
15 December 2016 at 08:07 #271939
David Jupp
Participant
@davidjupp51506
Free standing simulation of cut material – see CutViewer (only 3 axis milling), CNCSimulator, or MachineWorks. There may well be others out there.

Edited By David Jupp on 15/12/2016 08:14:09
15 December 2016 at 08:44 #271945
John Haine
Participant
@johnhaine32865
You might also look at G Simple – free to download CAM, can accept dxf input, or you can design simple things on-screen, it will generate and simulate g-code.
15 December 2016 at 08:46 #271946
David Colwill
Participant
@davidcolwill19261
Posted by Roger Head on 15/12/2016 01:31:38:

Having decided on Fusion 360, I will proceed to learn how to create component designs, and then (using the inbuilt CAM capability), create output files. At that point, is there any benefit in having, say, MACH3 without any mill attached? Will it usefully perform any sanity checks on the input file?

Related to that, is there any software that accepts the CAM file and re-creates a virtual component (on the screen)?

Roger

Hi Roger,

It wouldn't hurt to have Mach3 running unconnected. Whilst I'm not sure how much useful information you would get from it, I do think you would see glaring errors if you learnt to look for them. Mach has a toolpath screen that will give you an indication of how the tool is moving and also a table of maximum and minimum movements of X,Y & Z (very useful). The free version of Mach will be fine for this.

I'm not aware of any stand alone software that would display the part from G code and am not sure that I would trust one if there was such a thing. G code like any other language has dialects and it is often the little nuances that cause the problems.

One temporary solution, given your experience with steppers and servos would be to make a lash up machine which could be extremely crude given that it would be just to show how everything moves and check that nothing unexpected is happening.

Once you have reached a stage where the CAM program and Mach 3 are talking the same language the whole thing becomes very reliable and if anything stupid happens it will 99 times out of 100 be something you did.

David.
16 December 2016 at 00:40 #272110
Roger Head
Participant
@rogerhead16992
Plenty of advice, thanks everyone. I've followed up searches on just about every product and piece of terminology that has been mentioned, and I'm starting to connect the dots into a picture instead of a blur of information. Well, in theory anyway – I expect that practice will deliver the sound of misconceptions crashing to the floor.

In the blurb for various CAM programs the term 'post processors' comes up. I gather that these are to tailor the final output to match the requirements/idiosyncrasies of particular CNC machines. Fair enough, but this implies that there is an intermediate stage in the processing. Is that stage available as an output file, and is it in some standard format? Maybe plain vanilla G-code, or something else entirely? Is it useful?

One other question concerns detecting the extension of a tool bit after a change (or even at the start, for that matter). I guess one needs an electronic 'touch detector' at some predetermined spot within the workspace… I can think of a raft of questions surrounding this. Maybe someone could preempt them.

@David. Yes, it would be simple to hook up some steppers. Probably need some limit switches too, which means having the steppers actually move something, rather than just watching them turn. I think Mach3 is open-loop i.e. doesn't need feedback on position? (apart from limits).

I certainly have plenty to think about. Thank you.

Roger
16 December 2016 at 11:03 #272157
Anonymous
Posted by David Jupp on 15/12/2016 07:49:07:

There are also simple software tools which will plot the toolpath (e.g. NCPlot, or indeed the screens within Mach3). Not quite the same as showing the material, but may be useful nonetheless.

I use NCPlot on almost every G-code program I generate. Since it creates the plot from the actual G-code it tells you what the tool is going to do, not what the CAM program thinks it is going to do. The toolpaths and material removal graphics you see in a CAM program are what the program intends to do, not what the G-code might end up doing. My CAM program doesn't always generate G-code that reflects what it thinks it is going to do. This seems particularly true for 4th axis programming, but I have had issues with 2.5D code as well.

NCPlot is also a useful sanity check against typos when G-code is hand written.

Andrew
Author

Posts