Adaptive Slot Cutting

[reynolds087]

Hello, I am a complete newbie, and don't know what I don't know. I've tried to figure it out on my own without much luck. I would like to cut a slot using a series of progressive arcs similar to the slot cutting in Fusion360 when using an adaptive tool path. Is there a way to do that in FreeCAD? I've attached a screencapture of the tool path in Fusion360 for reference, as well as my FreeCAD project. The example tool path is using a ridiculous optimal load that my machine could never withstand just so it's easier to demonstrate what I'm trying to do.

With all of that said, here are the things I am struggling with.

1) Begin cutting on outside of the stock rather than plunging or ramping into the middle. Treat the slot as an open pocket where it plunges to full depth outside of the stock and then maintains a relatively constant load on the tool the whole way through the slot.

2) When I select the bottom face of the slot, it only seems to generate a tool path that would cut the edges. I am not sure how to signal to FreeCAD that I want to machine the entire surface of the face I selected. Based on the preview, it looks like it ramps into the center, and then just goes around the inside perimeter.

3) If I am using a 6mm end mill and trying to maintain an "optimal load" of .025mm. At least, that is what Fusion360 calls it. In that case the tool would always maintain a .025mm width of cut once it reached full depth. Since FreeCAD doesn't mention "optimal load", I assume this is determined by the stepover? In terms of percentage of stepover, I think that .025mm is .04 percent of a 6mm end mill? It doesn't look like you can define less than 1% stepover in FreeCAD. I think I can probably get away with 1% which would be a little bit over .05mm width of cut?

[GeneFC]

I played with your file for a while. If I set the stepover to 3% or greater then the usual adaptive progressive arcs work as expected. I do not know why smaller values fail

However, it is really difficult to understand the reason for such tiny values. The tool would be merely rubbing and the operation would take a long time. I do not use Fusion so I cannot say what might be meant by "optimum load". But something does not sound correct.

The depth issue is easily solved by setting the stepdown to a value equal or larger than the depth of the slot. Then there will be only a single layer in the gcode path.

At this time I do not believe the starting location for the adaptive operation is user selectable.

Gene

[chrisb]

If you look at a common "feeds and speeds" chart (example: https://uk.cncshop.com/pages/calculatin ... and-speeds) you see that already for a single tooth the chipload is far above your values. If you are not in the diamond grinding business it is sensible to to make the chipload not too small, because the chips take the heat off, and making it too small just causes wear on the tool.

There was recently a video posted with an excellent lecture on this, which I thought to have bookmarked, but I cannot find it.

[pathfinder]

There was recently a video posted with an excellent lecture on this, which I thought to have bookmarked, but I cannot find it.

Are you referring to this?

viewtopic.php?t=77793

Also, I think in OPs case, the optimal chip load is referring to the chip thickness, so you can't just divide 6mm by .025mm. The calculation is more complex and needs feedrate, spindle speed and number of teeth of the toolbit as inputs.

That being said,.025mm still seems pretty thin for a chip.

[GeneFC]

Are you referring to this?

viewtopic.php?t=77793

That is an interesting video, but Seco Tools is a premium supplier for high-end industrial operations that would refer to "Adaptive Milling" as "High Speed Machining". In other words squeezing the maximum productivity out of both tools and machines.

I did not get the sense that the OP has either tools or machines that would fit into the HSM category.

Gene

[reynolds087]

My problem is that I am trying to mill a very large slot in cold rolled steel, with a mill that is made from 4040 aluminum extrusion. Trying to do even .1mm (.004 inch) passes results in extremely noisy chatter and resonance (These new steel pieces are intended to replace the aluminum gantry that I currently have). With .025mm or even .05mm passes if I predrill some holes to reduce the load, the machine can just barely handle it without vibrating itself apart. That is why it is so critical for me to use a very small stepover. I noticed that even in Fusion360 it will not generate the entire toolpath. I can only generate about 50mm of the slot otherwise it just dies during the toolpath generation. So what I did is use the G55 offset and just run 50mm at a time and keep changing the offset.

[chrisb]

Are you referring to this?

viewtopic.php?t=77793

Yes, meanwhile it is bookmarked.

[GeneFC]

My problem is that I am trying to mill a very large slot in cold rolled steel

If I am reading you correctly the plan is to mill a 20 mm deep slot with a 6 mm endmill, in a single depth pass.

This will never work with any sort of gcode path at all. It is a big stretch to mill a full diameter deep, in steel, with a lightweight machine. Going to a depth of more than three times the tool diameter is bonkers, regardless of the stepover.

You might make this work by using a number of shallow cuts. I have no idea how many would be needed, but you could check the capability by making some trials.

Sorry.

Gene

[lgrfbs]

This is an excellent example of writing better code than letting the computer do it.

The code might look something like this:

Code: Select all

#100 = 1
WHILE [#100 LE 5] DO1
Call O11
#100 = #100 + 1 (Increase #100 by 1 each iteration of the loop)
END1


O11
G91 
G1 X-10
G2 X0 Y10 I0 J5
G1 X8
G2 X0 Y-10 I0 J-5
RTS

References for this post:
https://ncviewer.com/
https://www.cnccookbook.com/g91-g90-g-c ... ogramming/
https://www.cnccookbook.com/cnc-g-code- ... s-looping/

Of course, this has to be adapted to the control system you have in your milling machine.