Cutting Improvements: Ramp Down in Corners and Full Height Finish Passes

CAD/CAM Software Tips
1

I am experimenting with two strategies to improve the quality of the cutting:

  1. Ramping down the feedrate before making a directional change; and
  2. Leaving a small amount of excess material around the part and then doing 1 final full depth finish pass along the contour

I think both of these strategies can be accomplished using Fusion360. The rampdown of the feedrate is the easiest.

How to Rampdown the Feedrate During Direction Changes

  1. Do all of you 2D contour settings like normal.
  2. On the Passes tab check Feed Optimization
  3. I used the following values:

Maximum Directional Change = Any sudden change in direction greater than this number of degrees will cause the reduced feedrate to apply. This doesn’t apply to arcs or curves since those are not sudden changes but rather a series of very small rapid changes.

Reduced Feed Radius = Any arc smaller than this radius will cause the reduced feed rate to apply. 5 inches may not be enough, I might bump this higher.

Reduced Feed Distance = How far before the direction change or arc we want the sled to slow down. Again I might bump this higher.

Finally, be sure to uncheck Only Inner Corners

I need to spend more time with this, but at first glance, I think it is helping, it certainly allows me to use the faster 35 in/min for the rest of the straight cuts which seems to be resulting in a faster total cutting time.

How to do a Full Height Finish Pass

There are a few options here:

OPTION 1 A Full Height Finish Pass at the Normal Feed Rate

This one is easy.

  1. Do all of you 2D contour settings like normal.
  2. On the Pass Tab, you should have Multiple Depths Checked already
  3. Use the following settings:

Maximum Roughing Step Down = Set this to whatever you are comfortable with
Finishing Stepdowns = 1 We only want to make 1 finish pass
Finishing Stepdowns = With Rough Final checked and a Finish Stepdowns at 1, this does nothing. If you uncheck Rough Final, the final roughing cut will leave this much material left axially, or below the bit.
Rough Final = I recommend checking this, otherwise your final Finish Path has to both cut full height material plus some additional material at the bottom, I felt like this was starting to ask too much of the bit.

  1. In order to leave some material to the side of the bit (radially) so that we can creep up on the exact profile for the finishing path, you need to check the Stock to Leave button and set the following:

Radial is perpendicular to the axis of the bit, this is the stock we want to leave until the finish path. Be careful setting this too high as we are cutting the full height of the stock, so the material adds up quickly. Plus since we are at full feedrate, this can become an issue fast.

You will always have to zero out Axial Stock to Leave. If this has any value, your final finishing cut will not cut through the material all the way, which is not what you want.

With these settings you will get a single finish path a full depth but full feedrate.

The Finish Feedrate setting at the top of the Passes tab is ignored for setup, that is an annoying “feature” of Fusion360.

OPTION 2 A Full Height Finish Pass at a Slow Feed Rate

This sadly requires two operations.

This one is easy.

  1. Do all of you 2D contour settings like normal.
  2. On the Pass Tab, you should have Multiple Depths Checked already
  3. The Finishing Stepdowns in the Multiple Depths section should be zero. And the Rough Final box checked.
  4. You need to check the Stock to Leave and use the same settings from above:

  1. Save this Operation
  2. Duplicate this Operation
  3. In the Duplicated Operation, under the Passes Tab, uncheck Stock to Leave also uncheck Multiple Depths
  4. Under the Tool Tab, set the Cutting and Plunge Feedrates to whatever you like for a final pass 10 in/min is a reasonable place to start.

That’s it. This final operation will do a full depth cut at a slower feed rate. So far I think I prefer this style to the full speed final.

I am still playing with this and I need to really watch Ground Control to be sure that everything is actually functioning as it does in the simulation, but so far I like this setup.

11 Likes
2

one issue I see with techniques like this is matching the tool dimensions…

for example: the router bits offered by MaslowCNC store aren’t suited to finish 18mm ply in the manner described above because the cutting surface is shorter than the full 18mm (+ spoilboard offset).

its not that its a major problem, but one must take into account all the variables in play.

good luck and please report your results back!

3

Good point, I am still using the more expensive Diablo bits that have 1 inch of cutting length.

With the MaslowCNC bits, you would need to enable multiple depths in OPTION 2 and make sure that the stepdown is slighltly less than the cutting length.

OPTION 1 may not really be an option anymore in that instance.

4

Awesome work! Thank you for taking the time to share the techniques you are testing. This has been something I’ve wanted to explore for a while, but without using Fusion 360 I haven’t found an easy way. Maybe it’s time for me to switch.

I’m excited to see your results, let us know what you discover!

5

With the feed rate set in Ground Control, how does the Maslow board respond to feed rate commands in the toolpath? I guess a better question is: how does the F360 gcode differ when deceleration is/is not used?

6

As far as I know the G-code protocol doesn’t have any sort of acceleration ramping, each line can specify a speed that it will run at like G01 X10 Y5 F30 or something similar. Fusion might generate a bunch of small moves which gradually reduce the speed, or there might be a step reduction in speed. Just guesses.

7

I am not sure what you mean? I am not aware of a way to set the feed rate in Ground Control.

Correct that is exactly what is happening. Maybe my description is inaccurate, it sadly doesn’t step down gently from the feed rate. Instead, about a 1/4 inch before the end of a straight line, it sets the feed rate to the slower rate. Then when it arrives at the end of the line before starting the turn it is already moving slower.

8

I still think that should help! I had no idea these settings were available in Fusion. Great find!

9

I’m curious what you are using for post and how it is running. I have been running very simple instructions to maslow as I was running into problems with more complex code. How is it cutting @krkeegan?

10

I should caution, I really only got the final frame setup on Tuesday. So I am still working out many bugs myself.

I also only ran this once last night, but it seemed to be an improvement over prior attempts of the same piece. Particularly the slower feed rate in turns. I don’t have a complete conclusion on the final full depth cut, some of my errors on the roughing passes exceeded the stepover for the finish pass so it was not perfectly smooth. I have hopes the further improvements in my sled and frame will tighten a lot of this up.

As for post, I am using the Generic grbl post processor. It produces rather simple G-code, there are a few codes that ground control ignores, but it doesn’t seem to matter.

1 Like
11

Awesome work! Thank you for taking the time to share the techniques you are
testing. This has been something I’ve wanted to explore for a while, but
without using Fusion 360 I haven’t found an easy way. Maybe it’s time for me
to switch.

please do not depend on the CAM software to do this. It’s a useful tool for
experimentation, but doesn’t address the lack of acceleration support in maslow

I’ll repeat my statement that we need to look at using a fork of grbl to drive
the maslow, since it understands far more g-code and already includes
acceleration in it’s planning.

1 Like
12

I totally agree. I think a fork of GRBL is the way to go moving forward. I’m planning to do that myself as soon as I have the time (it’s a big project), but no need to wait for me to get it started!

13

about a 1/4 inch before the end of a straight line, it sets the feed rate to
the slower rate. Then when it arrives at the end of the line before starting
the turn it is already moving slower.

it’s still useful for testing. One thing to watch for, when it suddenly slows
down, is there a slight error from the sled swinging?

and does this actually make any difference in the corner quality? or are we
going slowly enough, with enough friction on the sled that it doesn’t swing past
where we want to be?

14

I totally agree. I think a fork of GRBL is the way to go moving forward. I’m planning to do that myself as soon as I have the time (it’s a big project), but no need to wait for me to get it started!

I think the first step is going to be some reorginazation of the existing code
to make it easier to extract the needed functions

looking at the code I notice that we still don’t have a 3d coordinated move
capability.

I’ll look at posting a ticket on that.

1 Like
15

Actually, neither am I. :joy:

I could have sworn I saw a feed rate setting in Ground Control… but I’m guessing I confused the makercam toolpath dialog with the Ground Control settings.

Though I’m certain I saw a request for a feed rate knob that would allow the user to speed up/slow down the motion. I suppose this would be implemented as a multiplier on the F values in the G Code. (or similar)

16

Alright, I spent some time tonight doing controlled tests.

The Short Answer

I am not sure either of these options did anything, but I don’t see much harm*. My tests are too small and simple, it is possible on a more complicated design that the benefits may be more apparent.

The Data

I cut three of the same pieces with the following settings:

  1. Cutting speed 35 ipm, Corners 15 ipm, Full Depth Finish .05 stepover 15 ipm speed
  2. Cutting speed 35 ipm, Corners 15 ipm
  3. Cutting speed 20 ipm

All had the same .18 depth of cut and 10k rpm. All were cut in the center of the machine:

IMG_20170720_195721.jpg3024Ă—4032 2.75 MB

They are the three cuts in the middle.

Piece One Ramp Down in Corners and Full Depth Finish

IMG_20170720_211541.jpg2851Ă—2138 1.86 MB

IMG_20170720_211605.jpg3024Ă—4032 2.8 MB

The edges of this one really do look much better. But the corners could still use some sanding.

Piece Two Ramp Down in Corners

IMG_20170720_212054.jpg2138Ă—2851 1.91 MB

IMG_20170720_212125.jpg2138Ă—2851 1.54 MB

It is hard to see in the photos, but there is some evidence of the changing speeds on the top edge. The edge is also more rough without the finish path, but it would be relatively easy to sand it up.

Piece Three 20 ipm Everywhere

IMG_20170720_212544.jpg2851Ă—2138 1.98 MB

IMG_20170720_212602.jpg2138Ă—2851 1.53 MB

I chose these settings because it takes about the same amount of time as the first piece.

The edges are still more rough as expected. But there is no evidence of feed rate changes.

* The issue

Piece one is about .080 inches larger all around. I could easily have made a mistake in Fusion360, but I thought
I was very careful. Plus I clearly saw the finish pass happen and it took off material and the setting was at .05. Anyways, there may be something going on here.

Further Testing

I should have done one at 35 ipm all around. I will try that tomorrow

1 Like
17

I’m curious; how many segments are in that roundover?

I’ve been playing with Sketchup and trying to figure out what a reasonable number of segments for a given radius are. I realize that’s going to depend largely on how critical the smoothness of the radius should be, but if I wanted an indiscernible curve with no visible stepping, how short should each segment be?

Any rule of thumb for that?

18

I tried ramping while cutting my aluminum last week and had some strange behavior. I wasn’t sure if it was the way I generated code, or the ignored code, but…I had to re do the cut. I’m interested to see what you find in your testing. Thanks for doing it!

19

Are those curves being cut with a G02 or G03 command, or are they not simple arcs?

20

I think those may not have been simple arcs, I can’t recall exactly. But I have since cut a number of parts with arcs and the gcode outputs with G2 commands which seem to work fine.