Printable View
Hiya every one,
I'm hoping someone can help me.
I'm new to cnc and learning.
Managed to draw a part finally and am looking to get it into gcode for mach3 but lazycam is suitable.
Here is my 3d part.
Simple File Sharing and Storage.
Could someone tell me if it works and what program it will convert to gcode in.
Many thanks.
Becky
I failed to open the file
Did you select download?
It openend for me and it seems to say it is a track plate.dxf file but it only opens with line number and text.
you can post a dxf file on the forum. Clive
Yep, it's a track plate, when you click on the link above it will open it in browser. Along the top it will have down load. Click this and it will download the file which will open in a dxf software
Yes I downloaded the file but I could not get AutoCad2004 to open it. Is this a 3D file? to convert to Gcode you will need a Cam program . ..CliveQuote:
Originally Posted by Rebekah_harper
Yes it is, I'll make sure what version I saved it as. I am using 2013
track plate 2004
this was saved as a 2004 version
I have opened it now but if you are learning cnc I think you will find that that part will be difficult to machine and I am sorry but is beyond me at this time. I think you will need a Cam program to convert it to gcode. But I am sure somebody will step in and help out. Good luck. ..CliveQuote:
Originally Posted by Rebekah_harper
Ok, thank you for trying.
Good thing is that I am gaining control of cad software.
Just need a cam program that will deal with 3d parts
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)
Phill
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.
Regards,
Nick
Problem with this approach Nick is the time factor involved, 3D toolpaths require a tiny step-over so cycle times will be high for the whole part. The best or fastest approach is to use 2D toolpaths for the simple bulk areas like the slots and flats then just use the 3D toolpaths in the areas that require them.Quote:
Originally Posted by magicniner
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,
Regards,
Nick
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.
many thanks
becky
Becky,
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,
Regards,
Nick
CamBam is quite a good introduction - it has basic 2D cad built in and is easy to understand what's going on. It's got a 40 session full feature free trial as well.Quote:
Originally Posted by Rebekah_harper
Yes I know this has I've Been using Bobcad for 6yrs now so I know it inside out, Unfortunately it's also why I know it's rubbish at 3D.!!Quote:
Originally Posted by magicniner
Erm sounds easy and all that but in reality it's not that simple at all and with 110 of these to make then you'll soon see why combining cutting strategy's makes sense when you see the real time difference.!Quote:
Originally Posted by Rebekah_harper
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.
@Jazzcnc hi Dean, long post but invaluable content! For us mere mortals following this with interest but no way to open the OPs original file please, if possible, could you post one if your Solidworks renders so we have an idea what this part looks like?
Always with the negative waves Moriarti :joyous:Quote:
Originally Posted by JAZZCNC
What version you on Jazz ?Quote:
Originally Posted by JAZZCNC
Here you go Irving and yes long post but how the hell do you try to explain 2D/3D Cam in 10 words or less. . .Lol Attachment 10547Quote:
Originally Posted by irving2008
Ah ah great Film and times precious in my world just like the gold in film.!!Quote:
Originally Posted by magicniner
Version 24 John but only because they upgraded me Free due to there skanking sales man promising one thing and delivering another with all my protests and emails ignored.!!Quote:
Originally Posted by John S
Right, now I see. Def 2D for the slots and flats and roughing out the curves, then 3D for the rest, any other approach is crazy IMHO.Quote:
Originally Posted by JAZZCNC
Only other comments I'd add is the need for a jig to allow part to be flipped accurately and, depending on the size, consider whether several parts can be machined as one then separated in one final pass, which would decrease overall manufacturing time.
Fixture or Jig?Quote:
Originally Posted by irving2008
A bit like the difference between cannot and may not but both important distinctions IMHO;-)
Know what your meaning has Fixture is very different to Jig and actually often a fixture holds a Jig.!!. . . but Neither are needed actually.?Quote:
Originally Posted by magicniner
Because the slot tops are all on same plane there's a flat surface for when flipped, if the outer profile is done at same time has slots then It's a simple rectangle so when flipped new work coordinates are taken from the corner and material lower surface. No special indexing or jigs are required. . . . The Difficult bit will be work holding and even then that's not too difficult has it can be held in vice or clamped from the ends.
Thou like Irving says because of it's small size then chances are longer lengths will be machined then cut to length.? . . . . . .That's how I would do it anyway.
Getting back to the OP's original request and stepping away from the Tangents this topic has spawned I've had a fiddle in BobCad Cam V25 Build 996
Before posting code I'll wait for preferred tooling size, advance per flute and spindle speed from the OP, but here's how you could get there -
1. import and reposition (translate) the model
2. Create a new layer and select it as active, then used Extract Edges From Solid to create a wireframe in the new layer, which can then be viewed satndalone by turning off the original layer (with the model in it).
3. Use Profile for the flat edge, select the line where the flat meets the vertical for geometry.
4. Use Profile to take the curved edge down to the upper vertex of the curved suface where it meets the vertical, select the line where the curved surface meets the vertical for geometry.
5 Use Pocket with outside edge lines set as dotted lines (allows the tool to pass the edge of the work) to make the operation Open Pocket for the two middle slots.
Now you're into the curved surface, you'll probably use a function requiring a Boundary and selection of the surface in the solid model layer to be selected as the geometry.
To make your boundary create another new layer, set it as active and use CAD Line drawing based on Extracted Edges to construct a Boundary for the operation, usually 1/2 the tool diameter smaller than the surface to machine.
When you Compute paths you'll get something like this -
Attachment 10570
CAM is a lot more in depth than I ever imagined before diving into CNC, I've missed out all the detail of selecting tooling options, top & bottom of work where required and multiple other options within the functions, hopefully the above shows why it's rarely the case that a request for G-Code from a solid model is met. There can be quite a lot of work for what looks like a simple job and it's rarely simply a case of feeding a model to the software and getting G-Code out,
Best Regards,
Nick
Personally if I had to make these and , big AND here, in this quantity I'd setup on a 4th axis and using a tailstock to support a mounting plate mill enough out to cut up into as many pieces as possible.
The flat parts can be done with normal milling cutters either lying flat or stood up and using woodruff cutters.
The curves sections which as causing all the problems could be cut with an old end mill or router cutter [ more later ] with one flute ground back for clearance and the cutting flute ground for the radius needed.
The cutter could be ground to a CAD generated cardboard template as these curves are just clearance profiles and not critical to microns. Commercial ones are often die cast.
The reason I mentioned router cutters is that they are usually straight flute and grinding a profile into a straight flute is far easier than trying to follow the helix on an end mill.
I'm betting that grinding a couple of cutters is far quicker than drawing and coding the same part plus the time saved over one pass as opposed to many small step passes makes this a dead certainty.
All the passes can either be run manually or under CNC but the code for the CNC will be just power feed type passes.
3D CAD / CAM has is place but often and especially when quantity is involved a couple of jigs and special tools will be more cost effective as regards time and cash.
John,
I agree in principle with the idea of a specialized cutter for the curves, and it would certainly be faster from a production perspective but as I have no idea of the size of the curved sections it's hard to say whether it's practical or not.
Without interrogating a drawing accurately I'd guess at 10mm rad but only cutting over about 6mm of material.
So guessing it could be formed onto a worn or old 8mm or 10mm cutter, possibly less.
Basing this on a dimensioned drawing I saw where the gaps between the slats were specified as 4mm.
Seen various 3d drawings but can't recall seeing a 2D end section drawing
http://www.model-engineer.co.uk/site...079/471654.jpg
The slots are around 4mm wide, a custom ground cutter is a very practical option, it's highly likely that a standard router cutter might be found and modified for the job,
Regards,
Nick
Edit - I should post faster but I'm watching a film on TV ;-)
My first thought was the same John about grinding a profile but to stay strictly to the drawing then 3 x Rad would be needed has can be seen from this end profile. . . If can't be changed then thats 3 tools to grind.!!Quote:
Originally Posted by John S
Attachment 10576
Base Could be done with 9 & 14mm ballnose with part on it's edge but thats then messing around with another clamping op and setup and not everyone has 4th axis.
Personally If I was doing them, Then For lower base I'd just shoot 9 & 14mm ballnose up each edge and flat mill up centre, obviously done horizontal.
For the other side it's obvious for slots but the round over then I would grind a tool I think. I'd also make them in longer lengths and cut to size.!!
This would be very quick and don't think it could be done quicker really.?
On that lower base there is only 10mm between the two radii, so if you stand the track on its side you could mill the whole of the lower side with one form cutter. Cutter would only be 16 or so mm long.
Becky want's 190 ??? odd so well worth doing.
Top done as you say.