Any Aspire users? Help needed for creating perimeter cut on boundary of component

Hey gents / gals -

I created a 15’ radius dish in Rhino, 24" x 24" x 1" thick to be carved out of MDF. I’ve imported the model into Aspire and created a roughing and finishing pass but cannot get a perimeter cut using the imported model.

Is there a way to select the outer edge of the model and then create a tool-path to cut the outside the perimeter?

As a ‘workaround’, I’ve created a vector at the same dimensions as my imported STL ‘15DISH’ file (scaling down the 3D model to 23.8" so I can use 24" square pieces of MDF to maximize materials) and created a perimeter cut on the outside of that vector. I’m wondering if there’s another way to approach / streamline this.

I’ve attached some screenshots of the rough / finishing pass (can’t upload the aspire file here).

Thanks in advance!
Mike





In looking at Aspire’s website, it appears that it can import Rhino .3dm files (maybe check which version it can import). If so, maybe it will work to export the 3D model plus the outer edge curve as a Rhino file - perhaps Aspire will pick up both and you will have your outer contour.

Aspire appears only to work with mesh models for 3D objects, unfortunately .stl is about the worst format as it doesn’t support anything like curves. If the above Rhino format export doesn’t work, maybe a .dxf might? It can handle both meshes as well as curves.

Lastly, if you must use .stl for your 3d object, maybe a second .dxf export from Rhino of only the curves you need can be imported to the same file?

I don’t know Aspire, but those are just the first things that come to mind to try.

1 Like

In the modeling tab there’s a tool to automatically create an outline from the 3D model. That being said, from my experience you might be better off creating a separate dxf from rhino as you’ll get a smoother curve than the one aspire (or vcarve which is what I’m using) generates.
image

1 Like

Good to know, Siemen. I found that function and tested it out. It basically repeated my method of making the circle vector by hand, but in one click. Good tip as far as it possibly not being smooth. I could see this being useful for boundaries that may be a bit more complicated. Thanks for the tip on simply creating a separate file from Rhino for the perimeter - I hadn’t considered that. Thanks for your help.

Interesting. Thanks for the tips - I’m going to try a direct import of the .3dm file when I do the 30 degree dish and will report back should it help anyone else down the road.

Good tips RE .stl vs .dfx - I didn’t realize the latter was ideal for importing more data such as meshes and curves.

I think I have all the info needed in Aspire as I just created a circle vector and a perimeter toolpath (more than one way to skin a cat, I suppose). However, I’m going to try a different approach for the second dish just to get some more methods under my belt.

As an aside, I took a look at the toolpaths (using 1/4" ball-nose for the roughing / finishing pass and a 1/4" EM for the perimeter cut) and the time is estimated to be 11 hours! How would you approach this in view of expediting the carve? I tapped into another forum and the consensus seems to be simply a larger EM (perhaps a 1" or larger Freud ball-nose) and then customizing the settings.

I’m interested if you have any tips to speed things up.

Thanks again.

Well, there are a lot of factors here:

  1. Max feed and spindle speeds of your machine, rigidity/vibration
  2. Type of material and finish needed
  3. Step-over (scallop height)
  4. Quality of the cutter

Certainly increasing the radius of the ball cutter will result in fewer finishing passes (assuming the same scallop height) but in my experience, in shallow dish-like forms such as yours, larger diameter ball cutters do not necessarily give a better finish - because the “dead area” near the center of the cutter (where the cutting speed is near 0 and there is little to no cutting edge) is larger. So it will be a trade-off.

11 hours seems completely off though, for a 24" diameter disk, I would have expected something like maybe an hour or two with a halfway decent machine. At max 0.4" (10mm) depth in MDF, I might rough just the center with a relatively large stepover parallel or circular pass, then go right to the finish cut. I’ll have to fire up my laptop with RhinoCAM to test.

Remember too, that if this is not a production run, you can sand the piece by hand to finish - 5 minutes hand sanding is usually better than 4 hours extra machining time to get a finer finish.

1 Like

I found vcarve time estimates to be inaccurate and stopped relying on them. The time depends a lot on the machine’s acceleration and stopping values. But your example seems very far off. Perhaps you your feed rate, step-over and cutting depth settings are off? Hard to tell without knowing which settings you’ve used.

Hey gents -

Here are some photos of the default settings. Bear in mind I’ve never changed these on a project so if they seem laughable, go easy on me :).

As an aside, I found both a 3/4" and 1/2" ball-nose ‘MasterCraft’ (Canadian Tire brand) router bit in my bone-yard… perhaps these would be better for at least the roughing passes? If so, I have no idea what the ideal settings would be for these.

20%20AM 38%20AM
IMG_1555

100" (~2500mm) per minute seems slow for MDF, I would normally program somewhere around twice that, between 4K and 5K, but depends if your machine can feed that fast. 12K spindle speed is also somewhat slow for wood, but if that’s all you got… Otherwise a 10% stepover seems OK for a finish cut.

1 Like

I’d increase the stepover of the roughing to at least 70 %. And for mdf I’d probably increase the pass depth of the roughing to at least the same as the diameter of that 1/4 inch bit, if not more. Is this your own machine you are running and you are just figuring things out on the go or is there somebody teaching/helping you how to do this?

Quick update -

I’m trying to set up the 3/4" bit for the roughing pass but Aspire is throwing an error. Initially I had the pass depth set to 1.1" (default) and thought this was the issue because my material is only 1". I changed this to half the diameter of the bit (.375") but it’s still throwing the error. Any ideas what I’m overlooking?

Also, I’m running the Shapeoko 3XXL with a Makita router if I failed to mention that.

50%20AM 06%20AM

Update - changed Pass Depth to .25" as per some advice from a FB member and this fixed the ‘error’. It also cut the job-run time down to 6 hours… still a long time but getting better!

Hey Siemen - This is my own machine (Shapeoko 3XXL w/ a Makita router). I’ve run a number of jobs creating jigs and v-carves for guitar making but have always relied (and been ok, to date) with the default values. The 11-hour carve time on this project made me dive in a bit deeper… time to start getting my head around customizing settings w/ F&S.

By the way, I finally did get around to testing this in RhinoCAM. Using a 16mm (5/8") ball cutter for a quick roughing pass (8mm (50%) stepover) and a 6mm (~1/4") ball cutter for a finish cut at 0.6mm (10%) stepover, I ended up with a theoretical approximately 2 hour machining time. Feeds were 3000mm/m for rough and 5000mm/m for finish - which were realistic for the machine I used to have access to at the school. It did have a 30K rpm spindle, so that helps with the faster feeds. I think the finish stepover could be even a bit larger (like 1mm) if one is willing to do a bit of sanding, which would reduce the machining time some more.

1 Like

Also, if your 3D geometry doesn’t have corners or details but is just a large 3D surface, you might be better of with the large bit for the finishing pass as well. For the same distance of overlapping (and therefore the same time it takes to mill) you will get finer details than using a smaller diameter. So you can increase the stepover (and therefore decrease the time it takes to mill) while still maintaining the same level of detail.


Image showing comparison between 2 different diameter of bits with the same distance from center to center. The smaller diameter bit leaves larger ridges than the bigger bit for the same time of milling.

1 Like

In my experience, this will also depend on the material and the shape. As I stated above, I have found that larger diameter ball-nose cutters give a poorer surface finish on nearly-flat areas. In the posted case, as the material is MDF, this may not be really visible so it will most likely work fine. If the material was more sensitive, like acrylic, I think the smaller bit with finer stepover would be the better option.

1 Like

Correct, I missed that!

Thanks for taking a look. I successfully cut the 30* dish with the attached settings. I was able to push the feed-rate as the machine was running using Carbide Motion’s on-board ‘in-situ’ feed-rate accelerator. At times I had it up to 200% and the machine seemed to be cutting ok. I set the spindle (Makita) to about 4.5 on the dial setting. I have the artwork / gcodes generated for the 15* dish as well and am just heading down to the shop to cut it.

I think the step-over was set a bit too ambitions for my first finish pass as it left a pattern kind of like corrugated cardboard. I decreased the stepover for the second finish pass and it got rid of my ridges from the first pass. When done, a quick scuff sand smoothed it all out .

I’ll post a photo of the finished product here shortly.

Thanks again to all who chimed in to offer advice and support!

Mike

14%20PM