Rest Machining Issues

I have this design:

I want to pocket out the larger areas with a 1/4" endmill which works the way I’m wanting it to (see next snip)

But when I want to come in and clean things up with a 1/16" endmill, it still leaves areas to be machined that I know can be cleaned up by that tool.

Any idea why rest machining isn’t working like I’m wanting it to?

Here is the file:
LOGO v1.f3d (371.9 KB)

Hi Stephen,

I looked at your file.
Since your last tool is a taper I see that you are staying away from the walls .053" to not cut into where the tapered walls will be. That makes most of the middle pockets too small to get into for the 1/4" endmill - since they are only .351" wide. There are only 2 pockets that it can fit.
To get the 1/4" endmill to go into those 2 pockets switch your ramp style to “helix” and set the “minimum ramp diameter” to .05".

The type of ramp will stop the cutter from getting in some pockets if there is not enough room to make the ramp move.

Also it seems that the rest machining on the next tool does not know how much “stock to leave” was on the first tool - so you have to add that to the “rest machining” tool diameter in the second tool.

In order for the second cutter to know that you have left stock to leave on the first cutter - you need to add the cutter diameter to the stock to leave x 2. So the first cutter stock to leave was .053 so x 2 = .106" . Add that to .250" = .356"
That is the minimum diameter to put in the “rest machining” diameter on the second tool. I would add .010 for a safety margin. So .366" in the “rest machining” diameter on the second tool.
I ran it that way on your file and it all cleans up.

For you to see what is possible to machine with a 1/4" end mill just start by turning “stock to leave” off and putting ramp to “plunge”. Once you see what is possible then start adding stock to leave back on ( I know you need it in this case ). See what pockets are excluded by that. Then turn ramp on and play with the various types of ramp and size to see what that excludes.

Hope this helps.


Hey Chris, this does help! I really appreciate you explaining that. I didn’t realize I needed to add the STL to the tool diameter. Thanks again for your help!


I’m having issues once again with Rest Machining. I’m just trying to clean up that lip (pictured) with a 1/4 endmill but I keep
BLANK 2 v2.f3d (84.3 KB)
getting warnings. Any idea how I can accomplish what I’m trying to do?

Hello Stephen,

Rest machining is a little odd in F360 (compared to other CAM packages I have used.)
It does not know or try to figure out how much stock is left on a model. It assumes every cutter mills to finish size.

So I see you added the previous cutter diameter and the ‘stock to leave’ together to get the diameter you entered in rest machining - 1.375" with no corner radius. And I know you want .125" left on the wall for the 1/4" endmill to finish. Unfortunately this trick does not help at all in this case.

F360 thinks you actually took a 1.375" diameter cutter and cut right to finish size against the wall. Since your wall on this piece is wide open ( no other intersecting walls ) F360 thinks the 1.375" dia. cutter finished it - so nothing left for the next cutter to do. That is why it will not generate a toolpath with the 1/4" endmill.

F360 does not know what your previous tool diam. was. It just goes by what you type in to the ‘Rest Machining’ box. For this reason I only use rest machining when nothing else will do it.

You could set the ‘Rest Machining’ corner radius to something like .250", a 1.375" dia. cutter with a .250" bottom rad cannot finish that wall. That’s why this trick works. If you try it you will see that does work but it does not really do what you want.

Better is to use ‘2D Contour’ toolpath and leave “Rest Machining” off. Hold down the ‘Alt’ key and select all the top edges of the wall. Turn on ‘Roughing Passes’ under the 'Passes" tab. Enter something like .06" in 'Maximum Stepover" box and 2 in “Number of Stepovers” box. When you turn on “Roughing Passes” a new option appears in the list above it called “Stepover”. This is the finish pass stepover ( I wish they would have named it that ). Set that stepover to something like .010"

The 1/4" endmill will then make a pass .070" away, then another .010" away, then the finish pass. Have a look at the attached I have modified:
BLANK 2 v2 better rest finishing.f3d (91.2 KB)

1 Like

This is great and thank you for explaining so well. It really helps when you explain how Fusion functions. Thank you again for your time and help, it has saved me a lot of headaches.

1 Like