Cutting tool recommendation needed

[Rob Davis]

With the forum being slow for whatever reason, I thought I'd ask for some advice on something.
Attached is a picture of our 5x10 table with parts on it. We make these for another company at 750 per month and we get 92 per sheet. You can see there is a lot of cutting here. We circle drill the 2 smallest holes with an upcut 1/4" tool, the 2 bigger holes with a 3/8 straight bit and the large holes with same 3/8 straight. We outline with a different 3/8 straight.
We can't use upcut on the outline as it lifts these smaller parts off the table and will fling them around if they come loose. We can't use compression either as we end up with a fire in the board, but that is another story.
Anyway, our issue is we only get about 3 sheets of MDF before we have to change outline bit as it gets dull so fast and starts to push parts around on the table when it dulls. Any suggestions on what to use with MDF that is cost effective? We're thinking about diamond but the price is high versus a 3/8 straight bit and we would have to see huge improvements to cost justify it.
Not urgent or a crisis. But advice is always welcome!

[Josh Rayburn]

What feed speed are you running your outline tool at?

[Rob Davis]

18000 rpm
475 ipm, but remmeber that it rarely gets up to that speed because cuts are at max an 8" straight line.

[Josh Rayburn]

double pass, first with a 3/8" up spiral, leaving .020" then cut the skin with a 3/8" downcutter
this will get the dust out, which is what kills the bits (heat) on mdf.

jnr

[Rob Davis]

Great suggestion! So obvious now that I think about it but couldn't see it. Could I increase from 475? We settled in there after breaking a bit but I think it was more due to heat and dullness than speed. A double pass on this will add significant time, more than a couple $ for a straight bit! But it would also help clean up on the table so save some time. If we coudl go faster, I might come out ahead. How fast can I feed 3/4 MDF??
I'll give it a try and hopefully remmeber to let you know.

[Josh Rayburn]

You can probably feed it up to 550 depending on the actual geometry of the tool and the grade of carbide, etc. but as you said, it won't actually reach that speed. The faster the better though. That will also help to decrease the heat buildup. You will get significant deflection so you may want to experiment first and move your first pass outside the line so your second pass takes the deflection off the part and cuts the skin at the same time. Let me know how you make out.
jnr

[Rob Davis]

Josh,
Tried it couple ways.
1) did it with upcut as suggested and then cut skin away with a striaght cutter. Originally had skin at 0.020 but it wasn't enough so had to go to 0.035 but not a big deal. Problem was the upcutter left a "fuzz" on the top part edge as you might guess everywhere the upcutter went. After going around the outline with the straight cutter, it was reduced but still there so we had to touch up every part to get rid of the ragged edge - easily done but extra anyway. Ideally I think that we would want an upcut bit that is slightly smaller diameter than the outline tool (straight cutter) so we could clean up the edge as we took out the skin. I was a little disappointed that the machine still left a bunch of dust in the grooves and we still had to clean up the table after the run. Extra outline step added 12 minutes.
2) Then we tried to run the thing just using the upcutter, leaving no skin, first pass cut through all the way. We had a couple "lift" off the table and move around on us but mostly we think this is the way we will go for now. It eliminated the second outline step so saves almost 12 minutes. Left about the same amount of dust as above but a lot less than our usual method, and the machine ran without bit vibrating, etc..

I plan to send the upcutter to be resharpened when it gets dull so it will get returned smaller diameter and then we will try the two step again with a full size straight bit and see if it works better.
Just for info, when we started the run, our vacuum was 27"Hg and by the time it was done, we were at 24"Hg. Not huge but interesting.
Thanks for the help!

[David Egnoski]

Why can't you use a compression tool for the outline?

[Rob Davis]

David, been there and done that and the issue is the tool gets too hot and burns the parts in MDF. THe dust generated is so abrasive and the compression bit packs it in there and the tools dull quickly and get way too hot. When they get hot, they dull faster and then break while cutting. We have had a fire on our table with this method (see previous posts regarding this). We use compression bits on plywoods and melamine without issue. It is just MDF that is our problem.
We even recently tried to use the 1/4" compression bit on the small holes and we had charred parts. (tool rpm is 18000)

[Will Williamson]

Has anyone tried single flute cutters on MDF ? I noticed they were on sale at MSC Industrial Supply. I am going to give them a try.

[Ryan Hochgesang]

My experience has left the single flute for plastic applications only, however it's always worth a try....... Another tool that I've found to work in multiple applications is a 3-flute, low helix type tool. Seems not to pull up as much on part as a typical up spiral tool and with 3 flutes seems to clear the way when removing chips and leave good edge quality. This has mostly proven good for harder plastics in my experience, but I would also give this a try in your MDF application to see...

[Will Williamson]

Has anyone tried running compressed air line inside dust hood to blow out extra dust so that when cutter comes around again it is not regrinding old dust . I know when I follow cutter with hand held air nozzle this works . On the other hand this additional air could cause parts to lift ? I have been looking at a cold air settup by Exair. It would serve 2 purposes excavate dust and cool the bit. Any experiments on Thermwood's part?

[Ryan Hochgesang]

There have been some general cut practices performed using the cold air on tool and yes this definetly helps significantly on cooling tool prologing tool life as well as chip cleanout. This works good with plastics to help keep chips from getting hot and gooping up in the cut path. I would think that in general it also helps blow the chips free and if a dust hood is covering the chips will be pulled through collection.

[DanFecteau]

If you could also find Ranger mdf it would help you a lot. Ranger is made 100 % soft wood, Excel is almost 100% hardwood, flakeboard is in between....so it is an important factor also !