Page 3 of 3

Re: downcut on plywood = fuzz

Posted: Fri Mar 11, 2016 7:39 pm
by TDA

Let me first be clear in saying I wasn't going after you or trying to single you out as being wrong. My intention was just to provide more information. I can understand how it was taken that way with how I framed the argument and using your numbers. My apologies. There is also the issue that none of us have a perfect machine, tool, spindle, material, etc. At the end of the day we usually have to compromise and find what works best for each combination.

That being said I feel I should address a few things you brought up.

I feel that the more things to go wrong statement is incorrect. At least as a general statement of deeper pass cutting. With a deeper pass you are going to have more issues with deflection, hold down, heat, more required torque out of the spindle and steppers, etc. If you are losing steps that's a separate issue that needs to be dealt with (although it may be from the higher torque). In general I feel it's better to leave these issues to those much more familiar with this system than me. Maybe there's a good reason for it with your system. In my experience though the above applies.

In most cases we have a number of things we can change to try and find a best possible combination to hit our chip load and stay inside our machines ability. Those typically are tool geometry, feed, RPM, and pass depth. Let me layout a few scenarios here. For the sake of uniformity I'm going to start with the same numbers we were using before and use the PDS chart (usually much better to get chip load data from tool manufacturers though).

So we are currently running 51 IPM (1295mm) at 30K with a 2 flute cutter. That gives us a chip load of 0.00085" (0.022mm). Our goal is to hit the minimum of the chart . There are a few ways we can do this. One previously discussed is increasing the feed. To hit our .003" chip load we are going to need to be moving 180 IPM (4572mm). At this point we may be exceeding a machines ability to keep up. We can reduce the pass depth and that will help some. But maybe we are still asking too much here for our setup. So let's look at our options.

Let's say we are using a Dewalt 611 (mostly because I'm familiar with them). With this router we have a RPM range of 16,000 to 27,000. So let's go ahead and reduce the RPM to the minimum. Now to hit our chip load we only need 96 IPM (2438.4mm). We will still need to reduce our pass depth. But, we will be putting less strain on the tool and most likely increasing tool life and cut quality. But what if we can't reduce our RPM?

Tool geometry:
Instead of using a 2 flute cutter we will switch to a single flute. This allows us with the original 30K to only need 90 IPM (2286mm). Again we will need to reduce our pass depth. And again we will most likely increase our tool life and cut quality. But let's say that isn't enough of a reduction in feed.

We could also look at reducing the tool diameter. As you can see in the chart your chip load numbers scale with your tool diameter. So let's keep a single flute cutter and reduce the size down to 0.0625". For the sake of argument lets say that the chip load scales linearly. So we need to hit 0.0015 to 0.0025. That would mean we would need to run 45 IPM (1143mm) to 75 IPM (1905mm). This will obviously take longer as we are working with a tool half the size. Again though we are looking at better cuts and longer lasting tools.

We can also look at the reduced RPM with the single flute tool. At the 16k with the single flute tool we only need 48 IPM (1219.2mm) to hit the 0.003". We could also run at 80 IPM (2032mm) and hit the 0.005" chip load.

Let me finish this by saying that all of the above being said I understand having to work in a less than ideal situation. It may end up that running at suggested feeds and speeds is not possible without expensive tooling or machine upgrades. That's not always possible or realistic. I'm just trying to provide more information for people to make their own decisions. Ultimately sometimes what works with what we have is the best option. But I would encourage at least keeping an open mind. Sometimes we settle for what works when there are better solutions.

Re: downcut on plywood = fuzz

Posted: Sun Mar 13, 2016 4:18 am
by DRobs86
No need to apologize. I am enjoying the discussion. You list some good info.

I will openly admit that my settings are non ideal. Before anyone bucks the trend and adopts my settings they should know that I usually am cutting items that dont require much precision. I am just interested in getting the work done quickly. I also think, without real scientific data, just casual observation, that the endmill wear due to too low a chipload does not outweigh the overuse of a small portion of the flute length. That said, I may benefit from the single flute. Ive thought about it before but never pulled the trigger.

I think we will have to agree to disagree on the relative risks of slow and deep vs fast and shallow. On the note of deflection, I think that we should consider a couple things there. Lets say you have a 13mm flute length and only cut with 1mm of it. Lets further assume that the forces acting on it (open to correction here) are the same whether zipping fast and shallow or deep and slow. The force is acting at the end of that endmill, versus being spread evenly along the bottom 6mm. Deflection increases linearly with force but with the cube of length. If these hold, your milling approach produces greater delection of the tool. Again, I am open to correction here.