Profile cutting advice

[christiangray3]

Greetings,

I’m running a PRT Alpha 4’x’8’ with upgraded control cards to run current Shopbot software. I’m using Rhino and Aspire for design and assigning tool-paths and G-Code.

I’m cutting 1” MDF into profiles, pictured below:

29063
29064

I'm currently using a 1/8” Amana 46270, 1/8” diameter, 2-Flute, up-cut spiral Foam Bit. I'm using this because the space between the "fingeres in each profile is 3/16". I already purchased (and used...I've built 1/3 of this piece already) the 3/16" acrylic that's going to live in between the fingers so I can't redesign at this point. I'm using the Amana 1/8" because the Onsrud 3/16” Super “O” was leaving deep machine marks (ridges) and sanding the pieces to a “finished” look was taking too long. I replaced the Porter Cable router, as recommended by a Shopbot Tech (I was getting large step-like grooves especially on one side of the profile cut, on each pass (machine marks) and it wasn’t cutting the line as accurately as it used to. I found the Amana 46270 1/8” with the 1-1/8” Cutting Edge and was hoping to use it to cut the profile is multiple passes and then run a finishing pass ("Last Pass" function in Aspire) to smooth out the machine marks and avoid a lot of “finish” sanding. Also, the smaller bit is more accurate in cutting the 3/16” “grooves” that create the spacing between each “finger” in the profiles. What do you recommend for the following:

1. I have a new Porter Cable router installed on the PRT Alpha. I talked with the Shopbot Tech and he recommended using 19,000 RPM for these cuts. Do you think that this is the best RPM for the job?

2. What feed rates should I use for this bit considering the material? I was told 5-6" per sec and start with at 4. I"m running it just under 4 right now using the Amana chip load calcs for 1/8" cutting MDF.

3. How many passes?

4. How much material should I leave for the “last pass”? (Should I leave an onion skin for the last pass?)

5. How much offset should I use in the “last pass” set-up feature in Aspire? (to hopefully take care of the machine marks left after each pass)

I’ve been experimenting and I’m running out of time and material to get it right. I've also snapped 2 bits in the process. Any help would be greatly appreciated!

Also, if there is anyone in the NYC area (I'm located in Greenpoint, Brooklyn) that is available for paid consultation, please let me know. I have another, more complex piece to cut after this one and could use some help from someone with experience in Rhino/Rhino CAM, Aspire, has been or is a Shopbot Operator. The next piece involves flip-milling 3D pieces out of 1/2" MDF. Essentially multiple angled Beveled-edges per four-sided planer, facet piece.

Thanks for your input!
CG

[guitarwes]

I'll try, I'm by no means an expert:

1. 19K seems a bit fast to me for MDF unless you're feeds are really really fast. (Will the PC router even turn that fast? I have a spindle so I don't know) I would back it down to about 12-14K and go about 4-5ips at 1/3 material depth per pass with a full depth last pass.
2. See above.
3. See above.
4. .05 on bottom
5. .01 offset conventional cut

[guitarwes]

"I was getting large step-like grooves especially on one side of the profile cut, on each pass (machine marks) and it wasn’t cutting the line as accurately as it used to...."


This sounds like your bit is not perfectly perpendicular to the table surface. Check to see if you have some lost motion in your Z axis.

[christiangray3]

Thanks for the advice, guitarwes! Much appreciated! The more I've researched this, it does seem that it could be an issue with the bit not being perfectly plumb, and/or issues with the table getting out of square. I'm going to test it today and tomorrow my new bits arrive so I'll be able to run some text cuts again.

I will run a test cutting the profiles using your suggestions and post the results.

Thanks again!

[Mayo]

If you're snapping bits you may be making your cuts too fast, or taking too deep of a cut, or a combination of both.
A common recommendation is to make your depth of cut only 1/2 of your bit diameter. This can be tweaked depending on the material you're cutting, the speed of your move and the depth of cut per pass. I routinely exceed the 1/2 the diameter of the bit recommendation but not so much with 1/8 inch bits.
Taking that into account if you want to cut 1" MDF with a 1/8 inch bit, you would need 16 passes at .0625 depth (1/16") plus your extra finish pass if needed. For your cutting (move) speed, I know this will sound incredibly slow but I would start at 1" or 1.5" per second and gradually move faster from there. I would make the router assuming you have the variable speed Porter Cable, at 12,000rpm and see how it sounds. If it sounds like it's bogging down then put it at the next faster speed and see how that sounds. IF you're burning the MDF then the bit is spinning too fast or your cut speed is too slow. If you're getting dust instead of chips you may be moving too slow but sometimes MDF gives dust no matter what I do...

If you have extra MDF to practice on, make test cuts (squares and circles) at various depths and move speeds and router speeds and write down your results for future reference.

[Burkhardt]

Such a long flute slim bit is inevitably prone to breaking and the usual rules for depth of cut and feed rates are too aggressive. As recommended earlier you should start with shallow cuts at moderate feed rates and increase until problems occur. 12k - 15k rpm should be reasonable.

But you can do yourself a favor and use cheaper bits to make the breakage less painful: http://www.the-carbide-end-mill-store.com/m5/170-2125--1-8-square-end-mill-extra-long-htc-170-2125-2-flute-gp-30-uncoated.html (assuming your router can do 1/8" shank...)

As for the offset you could try zero offset and do the layered cut in climb mode followed by a final pass in conventional. The bit deflection in and out of the material may already do the trick for removing the layer watermarks. If not you need some experimentation.

[christiangray3]

Thanks for your advice, and the link for the bit, Burkhardt. Much appreciated! I just ordered the bits and adapter for my 1/4" collet. I've been snapping the $42 Amanas...they add up!

[christiangray3]

Thanks, Mayo! I slowed everything down today and got better results. I was trying to optimize the cut times so that I could finish two boards in one day but that's not going to happen. I'll do some more test cuts tomorrow and hopefully dial it in.

[Kyle Stapleton]

I think you need to change how you are cutting this.
This is what I would do, make the spaces between the fingers a pocket and run that run that first with your .125 bit, after that make the rest a profile and run that with a .25 or .375 bit.