Disastrous first cut. Help in understanding what was wrong?

[eduwushu (Ed)]

Hi guys

Finally I decided it was the time to try cut the first strut for the machine. I did some tests before with the pen making sure everything was looking good and finally gathered the courage to put the bit and try the cut. But at some point everything went sideways and I have some guesses about why but I prefer someone with experience can maybe tell me.

First the setup:
I went to bauhaus and as i couldnt find mdf board as thin as 6mm I saw there was oil tempered hard board. Which was also a type of conglomerate and which I thought could be a good replacement. I guess this could have been part of the problem. So this was the working material

TROSSBOTTENBOARD LJUNDBERG FRITZOE OLJEHÄRDAD 6X550X1200MM

Then my setup in ESTLCam I used this tool with the parameters that are considered failsafe in the V1 website

For The Impatient¶

If you just want to get the machine dirty here is the generic recipe. This should work in every material softer than metal; you can optimize later.

• Single flute ⅛″ upcut bit.

• 8mm/s Feed Rate (The speed at which you move through the material).

• 3mm/s Plunge Rate (The speed at which you move vertically into the material).

• 1mm Depth of Cut (The thickness of material your bit will be removing per pass).

• 45% Step Over (The percentage of bit diameter that should be in contact with the material)

• Use the Peel pocketing strategy.

• Always use a finishing pass of ≈10% of your tools diameter. The denser the material the smaller the finishing pass.

So this is how it looked in ESTLCam

I used helicoidal drill for teh holes and the exterior i used the Part function leaving tabs

I attach the gcode that was generated

Then for the execution bit:

I used the 1/8” single flute carbide bit sold in the v1 shop. I have a Makita router RT0702C. And I put the speed dial to 6 on it

Now checking the manual I realized that corresponds to
Number min-1
1 10,000
2 12,000
3 17,000
4 22,000
5 27,000
6 34,000

34K rpm, which is a lot above the 24K that I said the tool uses in ESTLCam. Guess I should have gone for something in between 4 and 5

As for what happened:

The holes were done ok. And the machine started to do the whole outline of the strut. In theory I have a Z step of 1 mm so quite a few passes would have been needed
Already on the first pass at some point I started hearing a change in pitch in the sound of the router, to something of a much higher pitch which for me is a sign of the bit probably getting too hot. I lowered the speed to 5 on the go which now reading the manual again I figured out is a big NO-NO. But anyway the high pitch lowered down so I figured out I kind of solved the issue.
I noticed also this type of hard board when cut doesnt leave a clean valley like the mdf but the fibers spread and fluff up. After finishing the first lap and going for the second pass (so 2mm deep) the pitch change to really high, i noticed the machine started to get stuck (jumpy behaviour on the steppers) so that to me was a really bad sign and I went immediately to stop the sequence but in the time it took me to do it I could see a small flame come from under the bristles. (Yeah I also had the bristles on so couldnt see really what the router tip was doing, which for the first cut probably was another mistake)
After everything was stopped I lifted the router and what happened is that the bit was out of the collet and had lodged itself into the board at an angle like completely in. So somehow had came out of the collet. The plastic bit on the bit was partially melted (and now is loose). I cannot see the bit bent or damaged which is kind of a miracle. The collet though shows some signs of damage in the opening , but is not really crazy. Dont know if it can be an issue (image attached)
In the board I was cutting it seems the second pass was already cutting all the way to the bottom, as you can see in the images as well, which is strange cause it should only have gone as deep as 2mm (I checked this in the gcode as well). I dont know if the bit came somehow loose and sink more into the material, or was caused by too much heating when started to sink more into the material… Im not really sure. But that was kind of scary

Any help on understanding a bit more everything I did wrong?

Thanks a lot for the help

strut_plate_A_cut.gcode (80.7 KB)

strut_plate_A_cut.gcode (80.7 KB)

[Tokoloshe (Philipp)]

@eduwushu

So somehow had came out of the collet. The plastic bit on the bit was partially melted (and now is loose).

That’s the problem if you are going too slow, with too many RPM and only 1mm deep. The CNC is not making chips (I mean, it’s not going to do so in MDF anyway) or cutting enough material. This is needed to take care of the heat that is produced. You went slowly, not very deep and with too much RPM which makes the endmill heat up basically instantly. This leads to the collet losing grip and the tool slipping. Has happened to me before with a 6mm endmill in MDF. You should go much faster and at least 3mm in MDF to at least get rid of most of the heat.

@eduwushu

The collet though shows some signs of damage in the opening , but is not really crazy. Dont know if it can be an issue (image attached)

This is definitely going to mess up your tolerances, but since it’s a hobby machine it might not be that bad. If you figure out that it is, hit me up…
(Was that an Elaire collet? It looks pretty mangled up… O_o.)

[eduwushu (Ed)]

Ok so if i understood well the material of the board wasnt the problem. To solve this i should:

1.-Decrease router speed to the 24k rpm , in between dial setting 4 and 5

2.-configure the tool to move faster (dont know how much faster really, double? 50%more?),

3.-configure bigger z steps. So 3mm for example instead of 1.

Next time ill take the bristles off to see better

The collet is the 1/8 adapter sold in the v1 shop

Any tip on what are the signs to stop immediately the sequence and the machine? So i dont again reach the point where actual damage can be done? This was quite scary for me tbh

Thanks

[Tokoloshe (Philipp)]

@eduwushu

Any tip on what are the signs to stop immediately the sequence and the machine?

If you can see it cut deeper than it should.

I ran my LR with 1400mm/min and 3mm DOC in hardwood, the LR is much more capable than you’d believe.

Always with a full depth finishing pass.

[eduwushu (Ed)]

Thanks man appreciate it. Was feeling really under the weather after this, but now Im starting to feel the itch to go and try again

[Tokoloshe (Philipp)]

You can do it! Maybe start with a test square.

[Bartman]

Your feedrate (FR) is way too slow, so you are overheating your bit.

Rather than throwing darts to find the best feedrate (FR), speed (RPM) and depth (DOC) I think that you should do some research into the concept of Chip Load (CL). Determining a suitable CL for a given type of material and a given bit will give you the information needed to select FR, RPM and DOC (or at least a reasonable starting point).

Here’s a good introductory web page that discusses CL:

Chip Load: Guide for Beginners - MellowPine

Here’s a post in another thread that discusses CL:

Thinking about feeds and speeds

Here is a handy guide to the whole Chip Load concept… You should be producing small/medium sized chips. If your CL is too small (too slow FR or too fast RPM) you will be producing very small chips/sawdust, then you are “rubbing” (also will cause excess heat, burn marks, dulling of bit, etc.). If your CL is too large (too fast FR or too slow RPM) , your chips may be larger, and you may hear the router “bog down” This, and router bogging down. Recommended DOC for most specified CL is 1x bi…

For your situation (1/8" single flute bit, hardwood), recommended CL is 0.004 inch/tooth (+/- 0.001). Converting that to metric, CL is 0.102 mm/tooth (0.004 IPT * 25.4 mm/in)

CL = FR/(RPM * # of teeth) therefore FR = CL * (RPM * # of teeth)

The CL is rated for DOC = bit diameter, and that is a reasonable starting depth.

Because you are using a single flute bit, FR = CL * RPM. Select a RPM that is in the middle of the router’s range, so that you can adjust up or down if needed. Say 20,000.

FR = 0.102 * 20000 = 2,032 mm/min (round to 2000). This converts to 33.8 mm/sec (round up or down to 30 or 35)

If you want to try a bit slower FR, then lower your RPM so that the CL remains constant, but I find that the router loses some torque at lower RPM..

So, first of all, replace the bit with a new one, then try DOC = 3mm, RPM = 20,000, FR = 2000 mm/min. Listen for strain on the router, and adjust the RPM up or down one notch if needed. Watch the chips that are being produced, and make sure that they are not sawdust.

As mentioned, this is a starting spot, so you may need to adjust for different pieces of stock with different hardness (plywood is notorious for having variable hardness).

Hope this helps.

[v3juggler]

I find that for most of the materials makita set on lowest possible rpm is fine. I usually start at around 1000mm/min and then change to faster feedrate during job run, if possible.

On hardwoods I go higher, like around 3.

Of course I still get in trouble from time to time, but I hope this is just matter of experience (lack of…).

Don’t give up! You will get there soon enough!

[eduwushu (Ed)]

Wow this is really detailed thanks a lot. Compared to what you suggest the way i was running was definitely madness. No wonder was overheating

You think then i ruined this bit and i should get rid of it?

[Bartman]

@eduwushu

You think then i ruined this bit and i should get rid of it?

The magic 8 ball says… “Signs point to Yes”