Critique / optimise my Fusion file?

Hello, if anyone has a moment to check my fusion file that would be great.

It’s cutting Renshape PU on a standard machine.

I’d like to get the milling time down if possible.

Any thoughts welcome.

Hi @Theo,

I had a look and here are some comments for you to consider:

  • feeds & speeds for the first toolpath seem to be aligned with the recommendation for renshape from the wiki, however I think it was initially intended for non-adaptive toolpaths (regular pocketing). Currently, you are using a large stepover (optimal load 5mm, ~80% of the endmill diameter) and not too deep DOC, so your adaptive toolpath looks like a regular pocketing, and these F&S should be fine.
    • side note1, any particular reason to pick the very specific value of 21280 RPM ?
    • side note2, the old Shapeoko feeds and speeds chart recommended a feedrate of 75ipm at 19000RPM, so 1905mm/min : you can probably push your current feedrate to that value.
  • but, you may consider leveraging the benefits of adaptive clearing using a smaller stepover but a larger DOC, to minimize the number of passes (and hopefully reduce cutting time). I tried pushing it a bit and changing the max stepdown to 19mm, which is the max cutting length of the #201 endmill: the adaptive toolpath is down to 30min instead of 1h. Of course, 19mm DOC at 5mm stepover is a very large tool engagement but…this is only renshape, I would risk it to see if it works. If it doesn’t, I would keep the 19mm DOC, reduce stepover to 2mm, and increase feedrate to 2500mm/min, the cutting time then goes to 45min. Or something in between these two examples.
  • you have “rest machining” activated for that first toolpath, which is not useful (since there is no previous operation…)
  • you have slopes in the 3D object, so just using an adaptive clearing toolpath will leave you with steps. You probably need to add a finishing toolpath with e.g. a ballnose ending to get to the final result you want (something that looks like the 3D object in the model)
  • also note that all your inside corners will effectively have the radius of the#201 (1/8" radius), if this is not what you want you’ll need a second toolpath (this time using rest machining) with a smaller tool to get into those corners.
  • for the contour toolpath, again you might want to use a larger DOC (and reduce stepover: you can use a couple of “roughing passes” and let the contour toolpath do that for you) to do it in less than 14 passes.
  • misc:
    • your zero point is set in a very specific location, I wonder if this will be practical to zero precisely there when you start from a square block of renshape (where that feature to referenced against, does not exist yet). Why not just use the lower left corner?
    • toolpath computation takes forever (on my old PC) because the 3D object is apparently from an STL conversion. You could consider actually (re)modeling it in Fusion, that will speed-up everything big time.

Disclaimer: I have never had the opportunity to actually cut renshape myself (but if Winston’s video about cutting renshape on a Nomad is an indication, it’s very easy to mill, hence my adventurous recommendations). So take all of this as generic advice, experimentation will be key (as it always is).

Happy machining !


Thanks Julien

Yes, based on wiki. Renshape type materials do vary in density, I’m cutting, which is similar to many woods, e.g. oak in density.

Does this value matter as the spindle is manually controlled?

19mm DOC sounds scary! I didn’t realise with adaptive cutting I could go so deep. But as you say it seems the greater depth of cut is better than the large stepover for time.

My uploaded setting had it taking 1hr 40mins, not 1hr as you suggested?

Yes, I considered this, but time was more important.

I tried the pencil tool path, that seemed to be the best choice? But an 1/8 bit seems to make little improvement and ended looking poor. I’m not aware of any smaller bits? that would work deep, unless I got a new collet adaptor for less that 1/8?

Would this be neat and clean around the edges?

Does that mean I zero Z on the waste board, and then XY on the top corner of the stock? Because I can’t zero the corner correctly if not hovering on the corner?

Didn’t know that was a factor, the file is a Sketchup import I was given. Normally I use Rhino which imports as editable surfaces.

1 Like

Wow I sure hope it’s softer to mill than oak, or my recommendation is way off :slight_smile:

No it doesn’t, I was just wondering. Do you set it manually to 20.000RPM then ?

Here’s the link to the current state of the local project I played with, it has the 2mm optimal load adaptive, at 45min:

Ok. Just asking because the result looks like this with “my” settings:

I did not mean for the flat surfaces, but for the corners: no toolpath is going to help since the geometry of the 1/4" #201 endmill is what it is. I meant you can add a toolpath with an 1/8" endmill that will go and remove more material in the corners, making them “less round” (but still visibly rounded, just with a smaller radius). If the rounded appearance of the inside corners is not a concern, ignore that comment.

Going to a smaller endmill (e.g. 1/16th) will be difficult as they typically don’t have a long enough reach for the depths we are cutting here.

It should be just as good as the current contour with 4.5mm stepdown, and it might be better because smaller stepover = lower tool engagement = fewer opportunities for deflection/vibration = fewer tool marks.
The optimal solution to get perfect walls around the piece, I think, would be to use an endmill that has a large enough length of cut to do a single contour pass at full depth, but finding one that has 45mm length of cut would not be easy. Doing two passes at 19mm is the next best thing I think. Or maybe doing a spiral toolpath around the piece would work great too.

If you have an XYZ touch probe, zeroing on the top left corner is the easiest (sorry if I’m stating the obvious), just install the probe there overhanging the corner, launch XYZ probing cycle, boom you’re done.

If you zero manually, indeed that’s more debatable, I would probably set the zero to the center of the top of the stock (easier to locate accurately and draw a mark there)

1 Like

Thanks again Julien.

3.5 - 4 Makita

Just downloaded it and it’s 1hr 20. See picture. Could it be another setting in the machine time?

Yes, thanks, I did consider this. I didn’t have a flat 1/8inch at the time.

No probe. But the stock is already overhanging so I doubt a probe would have room. Stock is 420x500 cutting to 400x400.

The issue with using the centre stock is that will be milled away! So if I run a second tool or the machine fails I am unable to use the same point. Hence using a corner of stock that is not milled. As far as I can tell this is the best option - A fixed corner?

Oh did you mean the total time of the 1/4" adaptive and the 1/8" finishing ? I was talking about the 1/4" adaptive only, which is 45min :

for those settings:

What you could do in these circumstances is:

  • zero to the wasteboard/bottom of the stock instead. Then when the time comes for a tool change, keep X and Y, and re-zero with the new tool on the wasteboard, and only reset Z0
  • buy a bitsetter and it will take care of the tool change impact for you :slight_smile:

But as long as you are happy with that specific zero point, by all means use it, I was just curious why you had set it there, and you explained.

I think the issue is Rapid Feed setting in the machine time box? What is the correct figure? I am just selecting the 1/4inch.

Also, how do you get the times to show up next to the tool paths?

Mmh. Now I have a question for you too: where do you click to get that “machining time” window?
EDIT: oh right, it’s there in the context menu for toolpaths

I activated the “show operation machining time” option in the preferences a long time ago, and that’s the only time I ever check now:

Oh thanks. I think your Rapid Time is wrong. 3000 is mine. Mine seems to be accurate to how long things actually take?

So I checked this morning, and for some reason rapid feed in machining time menu was set to 30,000 (!) for me, yet I’m pretty sure I never modifed it myself since I was not even aware of that setting.
Anyhow, if I change it back to 10,000mm/min, the toolpath now takes an estimated 53minutes.

You can slightly optimize that by enabling “Both Ways” in the adaptive toolpaths parameters, then it’s down to 47min:

But there are still a fair number of rapids outside the material. It should be possible to create multiple local adaptive toolpaths (one by “sub-pocket”), and optimize that further. And then again, only a cut will show if the 2mm adaptive load can be pushed (back) to a higher value in renshape, and then the cutting time would go down significantly.

1 Like

Mystery solved! Explains our different times. I’m pretty confident 5,000 doesn’t match real world times. Haven’t upgraded CM yet. Will stick with 3000 for now.

1 Like

If you have the opportunity to cut this project or a similar one with LOTS of retracts/rapids, let me know what difference you see between the estimated time and the actual cutting time.

I measured the actual cutting time on a project of mine this week-end, and the Fusion360 estimate was within 10sec of the reality, BUT it had very few rapids, so that configurable value had no weight at all.

Estimated cutting time aside, if you haven’t already I think you should take a look at Winston’s recommended GRBL params (which happen to be the defaults now in CM 5.x) the machine just feels more “alive”, and rapids can be up to 10.000mm/min, which in a project like the one in this thread, will certainly help a lot.

EDIT: sorry, just saw in the other thread that you are aware of the 10.000 rapids in CM5. Ignore that last paragraph.


This one is already cut, there will be others!

So tell us, what feeds/speeds/optimal load did you end up using and how did it go ?

I cut it before this thread, sorry, as per the original Fusion file. Posted here as a test case to see how I can improve in the future.