Can any one test this part so I know if it the design or the cam software.
I tried BamCam but the part doesn't even appear.
I can open it up in Autocad and see the rail has been extruded but It appears there are no 3D faces, when DFX is imported into Artcam pro, (reads no 3D triangle data)
It opens fine in Solid works just the curved surfaces are not so smooth and made from straight lines. (Maybe meant to be that way.?)
To create this then I'd would do it mostly with 2D toolpaths and just use 3D for the curved surfaces. Depending on material then could even be done with all 2D toolpaths if profiled tooling was created or found, this would greatly speed up the cutting time.
Save it as .igs or .iges for import into a wider range of CAM software packages.
I've just used Autodesk Inventor to open & Save As a .igs and opened it in BobCad Cam.
I guess you'll machine in two operations, the grooved side first and arrange a fixture or vice jaws that will hold the part for machining the second side.
To produce G-Code at least your tooling diameter and tip form ( flat, ball, flat with radius) with RPM, number of flutes and feed per tooth (both linear and plunge) also initial stock size would have to be defined in the CAM package to allow path generation for your machine.
I'm just clambering up the CAD/CAM learning curve but it looks to me as if you should be able to generate paths to cut the part with some fairly basic CAM functions, by defining a rectangular border to limit tool paths you could use most roughing functions and a surfacing function for both the slotted and the simpler side.
The Cam software used will mostly dictate how this is tackled but has you say creating a boundry area around the area required is often used. Again dependent on Cam software then you may need to allow extra for tool diameter.? Better more expensive Cam packages will do this for you but most don't, Bobcad Cam doesn't I know that for sure has I use it. ( Not for 3D thou has it's crap at it.!!)
In BobCad Cam you can define stepover and cut depths for most of the 3D paths allowing you to trade off finish against time as required, the precise solution will, as you say, depend on the package chosen to do the job with.
If I was making the track plate in the model I'd probably do it on my Emco FB2 and machine it manually,
well I am trying to give BobCad a go but the demo isn't installing.
however, I really don't want to over complicate things by combining 2D and 3D. I am happy to sacrifice time as I have plenty of it. at least I am not trying to do it manually 110 times as that would kill me.
so I am trialling feature CAD at the moment whilst I am trying to resolve BobCAD issues. The idea is to learn CAD and CAM at the moment whilst I build my CNC machine.
sofar I haven't generated any code yet so I am still keen to know if it will. if any one whats to give it a go to actually produce one that would be awesome to see.
thank you for the information so far, lots of food for thought.
as I need to do this in two stages, what would be a good method to set this 2 stage system up.
If you have no time pressure it's worth going with some trial installations, I tried this route but found that trial periods are aimed at experienced CAD/CAM users or those with enough time to learn and explore the software fairly well in the trial period.
You're also sure to get good help and opinions/recommendations for free software here, on the Mach3 forum and on CncZone forum, I bought my package based on price, it's ability to do what I needed and the excellent support and training materials provided,
Last edited by magicniner; 31-10-2013 at 10:59 AM.
Problem is that parts of your model don't suit 3D strategy's and tooling, for instance the slots have sharp corners and for an acceptable finish you'll want to use ball-nose cutter, this will put a radius in the corners. To remove this radius will then require additional operations and cutting strategy and often the cheaper Cam software's don't provide these strategy's, in this case called Rest milling.
Rest milling goes around with different size tool and removes areas that get missed by the previous tool, in your case you'd use flat bottom end mill to cut the radius away.
If you haven't got these more advanced strategy's available then your stuck with the radius or getting creative with what strategy's you have available.
Then there's the wasted time to consider, to get best finish quality with 3D paths and ball-nose tooling requires very small step-over's and has the tools get smaller in diameter the step down has to be kept lower else the tool snaps meaning multiple passes.
Getting round this tool stressing and multi passes problem then involves first using roughing strategy to remove excess material which again involves more time. So now you have 2 operations, 1 x roughing and 1 x 3D both these have to cover the whole surface area.
Then you'll still be left with the radius to deal with.!! So Even with Rest milling or other advanced strategy's like pencil milling your into 3 operations that have to cover the whole surface area. If you don't have these advanced strategy's then chances are your workaround will involve more time.!
Now if you combine 2D and 3D strategy's the operations get much simpler. The slots are simple 2D pocketing strategy's and because you can use straight tooling the corners are sharp requiring no clean up and can be cut in full depth and in one quick pass.
Same with flat areas which are simply done with area clearance or pocketing operations with same flat bottom tool and taking 50%+ Stepovers at full depth so again very quick.
This then just leaves the curves which are done with 3D strategy and roughing passes but now the area to cover is much less and confined just to the curves.
Because we have been using wider flat bottom cutter for 2D operations we use same tool for rouging. This then just leaves one tool change to ball-nose cutter which only has to machine the curves and blend into the flats.
Combining strategy's is not complicated and it's simple case of looking at the part and identifying the areas which suit 2D or 3D strategy's best then selecting the area by either defining a boundry to stay within or selecting geometry or surfaces. The Cam software you use will mostly dictate how this is done and how simple or hard to do. Better software makes this easy as clicking the surface or edges and it works the rest out for you. Others require you define a boundary calculate and apply offsets for tool being used.!!
The fact is Most parts like this require multiple operations to achieve a finished part. Combining 2D & 3d strategy's is no more complex or difficult than having multiple 2D operations like Drilling, pockets, profiling etc in one G-code file and something you'll need and want to learn quickly if doing these types of parts has the time savings are huge when doing multiple repetitive parts.
Hope this makes it clearer and don't be scared off with combining operations has it's bread and butter stuff that you'll need to learn and can save many hours or days work.
Last edited by JAZZCNC; 01-11-2013 at 01:46 AM.
By jcb121 in forum SolidworksReplies: 1Last Post: 20-10-2012, 01:50 PM
By RLKS Rob in forum Artsoft MachReplies: 2Last Post: 12-08-2012, 12:30 PM
By crossleymarko in forum CAD & CAM SoftwareReplies: 16Last Post: 21-04-2012, 11:45 PM
By Kai in forum General DiscussionReplies: 10Last Post: 14-12-2010, 06:07 PM
By scotty in forum Programmers CornerReplies: 3Last Post: 07-03-2010, 11:48 AM