Hi Guys,
I currently do a lot of 3D printing and Laser cutting. I work with many programs and as the title says my main Cad program is Solidworks. I just placed my order for the X-Carve and was curious if I was able to use Solidworks with it. As I am a newbie to CNC I am not sure, I’m guessing I can export it as a SVG but that never seems to export very well as far as curves. Any thoughts.
Brian
Hi Brian,
Thanks for ordering an X-Carve. To use Easel right now we only support SVG import. You can use Solidworks and another CAM package like HSM Works or similar and then export g code. You can then use a program like universal g code sender to send the g code to X-Carve.
I am using SolidWorks as well (just setting up GCode right now, for when my X-Carve arrives, and I am using MeshCAM to generate the code from the models. Everything works very smoothly so far, the code looks good, and the universal G-code Sender picks it up nicely.
… Can’t WAIT to get the machine, so I can start running this stuff! 
I’m using Solidworks too and then into Mastercam.
My code simulations are looking good so far, I can’t wait to try it out for real ! 
Cool, I’ll have to look into it. Anyone have any youtube tutorials?
I’ve been playing around with Solidworks for a few days now. Currently importing into Aspire (CAM) and then exporting as G code. I don’t know much about either programs so am having a lot of trouble with 3D designs. 2.5D is easy with aspire.
A couple of good resources for (paid) training tutorials in Solidworks -
I’d try Lynda.com first - Online Courses, Training and Tutorials on LinkedIn Learning
Digital Tutors have some great stuff available too - http://www.digitaltutors.com/software/SolidWorks-tutorials
Thanks David, bit Solidworks I’m ok with. Never used the Cam programs. CNC newbie
I have been using nothing but Solidworks and HSMxpress for my aluminum milling and it is a great combo. I do run a TinyG on the Shapeoko but HSMXpress outputs gcode with little effort and allows full control of 2.5d toolpaths with ease over all. I have done a fair bit of rather complex 2.5 d milling on it and it has turned out great so far. With a little bit of online reading you can get going with CAm in HSMXpress pretty fast. The level of control it offers really allows you to do some great milling jobs in aluminum.
Wow, impressive ! I hope I can produce something that looks half as good as that
Amazing work! Did you do the anodizing yourself as well?
I’m a complete newbie and learning to use Autodesk Fusion 360. @Travelphotog I really like what you have done there looks great. Awesome looking E3d mount. Once I get up and running with my X-Carve, I need to design an E3D mount for my 3d printer.
@Travelphotog those parts are gorgeous. Can you please tell us about your toolpath strategy? Is it helical? Do you use graduated plunging?
Thanks! With a little work the Oko can do a fairly good job in aluminum. I will be glad to answer any questions you might have on aluminum milling with the Oko.
Yes, sir! Everything is done in house in my spare time. Anodizing the parts is lots of fun and pretty easy if you stick with 5083 or 6061 alloys. Avoid the 7000 alloys though as tbey do not anodoze near as well. I also have small batch (2 Gallon) anodize dyes if folks wqnt to try thier own hand at anodizing.
I am flying out for my weekly shoot. When I hit the hotel this afternoon I will give you guys a run down of the toolpaths for the main mount. Sound good? Wheels up for now!
Travelphotog : those are serious parts, my friend ! Awesome !!! Kind of make me feel a lot better about buying a full set : finally something i’ll call “serious project class” ! I was genuinely worry that those kind of machine were limited to “simple” project. You also mentioned “home made anodizing”, if i’m correct, could you elaborate, please ? Thanks
Hey TotoTiti,
Thank you for the kind words on my work. With a little care and some measured DOC toolpaths the OKO can mill up to 1/4" (6.35mm) 6061 aluminum with ease over all. A few ponters: make sure you are JUST touching your work surface as you start the cut. Being off even .1mm can cause too deep of a first cut and induce chatter or even break a smaller end mill. I started out milling at .1mm DOC with about 65mm/m feed speed on the 3mm end mill. I have managed to work my tool paths such that now I am able to cut at .20MM DOC at 150MM/m feed rate on the same 3 flute Destiny end mill and great results. On smaller end mills like the 1.58mm one used on the screw tap bores, I slow down to .15 DOC and about 75mm/m feed rates. In aluminum milling on the Shapoeoko nothing good happens FAST. But if you take your time and allow the tool to cut instead of forcing it, you can see the results above.
As for the anodizing… I do all of my own anodizing after learning it last year for a large project. Over all you need a cheap ($50-100) lab power supply for DC that allow you to control the amperage and voltage. Sulfuric acid and RODI water (this is a MUST) are mixed to produce the needed electrolyte bath. A large surface area cathode is placed in the tank (large sheet of soft lead or titanium mesh) and the negitive current source is linked to it. Then a rod of titanium is placed across the tank and the postive current outlet is linked to it. Then titainum wire is used to attach the aluminum parts to the anodized to the postivve voltage source. Then a bit of math comes into play to set the right power setting and length of time for the anodize. Overall once the aluminum has a good anodize layer on it there is a slight “golden” look to it compaired to a none anodized part which still looks bright silver in color. These process is done at room temp over all for normal anodizing. Once the part has a thick enough layer built up on it (that color change we spoke about) you remove it and wash it in more clean RODI water for a few minutes to remove all the acid (or dip it in Nitric acid for more advanced anodizing) once washed the part is placed in a dye bath which is normaly around 140F. The time in the bath varies greatly due to which color you choose and how intense of a color you desire. Some colors need only a few seconds or a few “dips” while others need half an hour or more (the Nitric acid dip reduces this time greatly). The part is then “sealed” to lock in the color and protect the finish. I use a “boil” sealer in which the parts are boiled with a Nickel Acetate Sealant which I find works very well for my uses. Overall it is an easy process and one which almost anyone can do as everything is store bought and easy to come by. Though small batch powdered dyes are hard to come by as most suppliers want you to buy 30lbs or so when only grams to a few ozs are needed for a 2 gallon batch of dye color. (I do have a source and resell from time to time). Great care must be taken to clean the parts of ALL greese and things of the like. Even the smallest lapse in cleaning and handling will show through to ruin and distract from the finish of a finished part. That is a very basic overview of the process, though more is involved for a truely good finish from batch to batch. I am simply a hobby anodizer who has had lots of practice and much good luck. But with a little research anyone can follow the same steps and push their projects to the higher level of custom anodized finishing at home. Tapped this out on a flight home on a bumpy flight so please forgive me if I missed an error or two above.
Whoha !!! That’s a lot to digest ! Sound like a wealth of information. I have to say that anodizing is very intriguing, but will require careful planning, special due to a 4 year boy running around. Thanks again !!!
Sorry for the delay in my promised reply Mr. Kaplan. But as promised here is a bit more info on my tool paths. I hope I do not bore anyone to tears! As a side note guys, I am on a bumpy flight home from Detroit to Houston so please forgive any minor typos.
The mount needs 3 end mills and 7 or 8 tool paths to make. I use a 3mm 3 flute Destiny Tool end mill for the heavy cutting, a 1.58mm 2 flute end mill for the notch and the boring of the tap holes for the inner screws, I finish off with a 3mm 45 degree 4 flute Chamfer mill.
I first clamp down and mill a scrap spoil board flat with a 2 flute 3mm fishtail end mill. This makes sure the stock is 100% flat in relation to the mill. I use wide double stick tape to attach the Alca 5 tool plate 5083 aluminum to the freshly milled flat spoil board. I then load the 1.58mm end mill and attach a lead to it and one to the aluminum stock then perform a g28.2 Gcode command on the TinyG controller. This drives the end mill down to touch the surface and connect the leads whihh stops the Z axis on contact (almost). The controller stops the spindle, but not before dropping a TINY bit more then it should for true 0. So I send a g28.3 Z0 command to ZERO out the Z Axis, then send a G0 Z.375 followed by a G28.3 Z0 command. This raises the end mill up .375mm to allow for the “over run” fof the spindle dropping a fraction of a MM after making contact( I arrived at this number by testing and found it to “start” the cut at a true 0 for my setup). I then raise the Z axis to Z5 and start the first tool path for cutting the pass through on the mount. This is tool path is done in HSMXpress as a 2d contour with runs at .15mm DOC, 75MM/M feed rate and a 2 degree ramp in starting at .25mm above the surface. As each .15mm layer is cut down, it plunges the next .15mm down at 15mm/mm then makes the cut at 75mm/m. Then 2 finishing passes of .05 mm are run at full depth of cut at 75mm feed rate. then a third and final finishign pass is run at 45mm/mm.
Next the 1.58mm end mill runs a boring tool path to cut the holes on the inner lock ring screw holes for an M3 tap. This is run as a spiral bore path at .15mm down cut at 75mm/m feedrate. This is a rather fast bore so I might suggest starting out slower.
Next the end mill is changed to a 3 flute 3mm Destiny Tools VIPER end mill. The smae zeroing out process as above is used to reach a TRUE 0 above the work.
The next tool path cuts the main outer screw recesses. It is a bore tool path at .2mm DOC and run at 75mm/m. It again runs a spiral cut at .2mm DOC. Thhis produces a shallow recess in each of the three screw locations to hide the screw heads.
Next the same end mill is used with the same type of .2mm spiral bore cut to mill the screw holes to M3 pass through specs. This tool path STARTS just above the surfacce of the recess, but below the level of main stock to reduce air cut time and speed the tool paths along. care must be taken to make sure clearance height is allowed above stock level when moving from one recess to the next. The spindle is then moved to Z50 X0 Y75 to allow for tool change.
A 4 flute 45 degree 3mm chamfer end mill is inserted and zeroed out in the above method. Then a chamfer tool path is run at 55m/m then followed by 2 finshing passes at full speed then a third one at .45mm/m for a final smooth finish. Then the spindle moves again to Z50 X0 Y75 and Small #2 wood screws with custom milled washers are installed in the holes of each mount to lock them in place for all tool paths to follow. The 3mm end mill is placed back in and then zeroed out again.
Then the hotend recess bore tool path is run with same 3mm end mill. This is again a spiral bore tool path. But it is run at .2mm at 135mm/m. This is a faster cut due to larger size of the 16mm bore being milled. This cuts a 16mm 3mm wide recess in the stock. This will produce the needed space to hold the E3d heat sink for the mount. Again 2 finish passes are run at full speed and then a third run at .75mm/m.
Then the main cutout 2d contour tool path is run at .2mm DOC and 150mm/m feed rate. This frees the mount from the stock which is held in place by the #2 wood screws. The cut passes .2mm below the bottom of the stock. This tool path has 2 finishing passes of .05mm each at full depth run at full feed rate, then a third at .75mm/m for a smooth finish. The spindle then moves to Z50 X0 Y75 for a tool change to the Chamfer end mill.
The main outline Chamfer is run at 55mm/m then has a final finsihing pass of 40mm/m for a nice smooth finish. The chamfer tool paths are by far the hardest to program and cut. Even the slighest shift in the work will ruin a chamfer toolpath and your piece. It is for this reason that I run them after the last step of each tool path which i wish to Chamfer innstead of runnig all the Chamfers at the end in one tool path. The belts drive system of the Shapeoko just does not tend to produce a fine enough finish if a chamfer toolpath from several steps in run only at the end. I have found much better results by running the Chamfering tool path after each toolpath which i desire a Chamfer on.
Overall that sums up the toolpaths used to make my mounts. All my 2d contours are run without lead ins out lead outs and most have a ramp into them from .4mm above the surface to be milled. All the bore tool paths are spiral boring paths at a given DOC down cut. Care must be taken in reducing feed rates for smaller (narrower) end mills and tighter bores. Too deep of a DOC at too high of a feedrate might cut without breaking on a Shapeoko, but you tend to get a slight oval shape instead of a desired circle. While the same tool path at a slower feedrate wih give a “true” ciircle. Calibrate the Shapeoko often if it mills deep DOCs or higher feedrates in Aluminum. The belts so slightly drift a bit over time and need adjustment and watching to keep things where they belong and help you produce the same results week to week in aluminum. This is done with a dial indicator mounted to the spoil board and measured off the spindle shaft with it off. Command the spindle to move 1/2" towards the dial after zeroing it out on the spindle shaft. Adjust the belt tension and controller settings to make sure you get a TRUE 1/2" on the X and Y Axis… Removing the spindle and mounting the dial to the Z Axis will allow you to do the same for it which is VERY important for milling aluminum since DOC are so very shallow in aluminum milling on the Shapeoko… Also always mill a scrap spoil board for aluminum milling to make sure your stock is flat to the spindle plane. This one step alone along with getting a TRUE zero after each tool change will mak aluminum milling much easier for anyone wishing to give it a try on the Shapeoko.
