Yes, that's a 3-d tab.

I am a bit late on reading this thread.
I run a 2.2kw water cooled spindle.
I skim my board ( 2440 by 1220 ) with a 40mm dia cutter. 9000 rpm 7500mm feed rate 1mm depth of cut. Sure makes a lot of dust if the extract is not switched on. ...lol
I use 3d tabs 90 percent of the time. 5 percent is onion skinned. 5 percent i forget and make a right mess of things ...
Cheers Andrew

Wasn't really sure where to put this post...so I thought I would throw it on my build thread.
Does anyone here know jhiggins7 (John #26)? I haven't heard from him and have not seen any posts from him in quite some time. Just hoping he is ok?
He helped me out with a project awhile ago and wanted to let him know how it all turned out.
Thanks
Mark

His last activity on the board was today. Have you tried sending him a PM?

Yes, glad to report that I have heard from John. Sounds like he is doing well.
Mark

Looking for any advice!
I have to make some parts, 1 1/4" to 1 1/2" thick. I can use plywood, pine, mdf or really most anything paintable. I have some 1 1/4" mdf, but not loving it. Tons of dust, hard on bits (unless I am doing something wrong)? Of course I want to use least expensive material, do as fast as possible, etc. I could use standard construction grade 2x6's, knots and edge finish is not important. Any thoughts, on material and corresponding bit size, speed and feeds would be greatly appreciated!
Thanks
Mark

Use the chipload for the type of material from the manufacturer and start by using the calculated lower end feed and adjust acoordingly. My preference is solid carbide bits or carbide insert that are brazed on. It does not need to be a top of line bit but better than your El cheapo ones. MDF is dusty but you should be getting descent sized chips and not dust, if not, the dust will wear down the cutting edge. That is true for all cutting. That being said, MDF will have a shorter tool life but you could always use a burr bit, as some guys have reported good results with those. As far as what to use, indoor, outdoor, stability, longevity, 2D, 3D. .. you need to take all into account and go from there. You do not have any of that listed so we would not be able to answer you.

Thanks Pete
I have not worked much at all with MDF. I am getting mostly dust, not chips? I was cutting 3/4" MDF, using a Whiteside 1/2", up/down compression bit (can't find any info on chip load). I was cutting at 16,000 RPM, feed at 100 ipm, 0.220 depth per cut. Any thoughts on that, perhaps to slow on the feed?
This is an indoor project, making craft angels. Pretty simple cut out shape that is getting painted. I suggesed MDF thinking it would be easy to paint, but not having worked with it (except for just some basic cutting on a table saw). Perhaps using 2x pine would be a better choice (unless, I can get the MDF going)? The old supplier for this passed away, and I am sure was using 2x pine cut out on a band saw. Also FYI, I have a router (no spindle yet) , RPM range of 10,000 to 23,500.
Thanks for any input.
Mark

Now this will not be exact for your bit but they have an up down spiral which is the 60-100 series I believe. Double check it, don't take my word for it.

http://www.onsrud.com/xdoc/feedspeeds

Using the formula they give and like I said start at the lower end is best. Another thing to notice is the temperature of your cutter after the cut. If it is more than warm to the touch (a little above room temperature), your feed/speed is wrong. The heat should go into the material being removed and not the cutter. I don't usually go over 12k RPM with MDF but it is all about the machine so others may be able to run faster and not have chatter on their parts because of the rigidity of the machine and quality of the bit.

A lot of people think run the speed faster and the machine slower is conservative but it will destroy a bit as fast as speed too slow and machine too fast. It all has to match.

You will find that with chipload or IPT (inches per tooth) that most manufacturers don't give them. So once you find a good chipload and long tool life for that tool, be sure to write it down. You can always call the manufacturer and ask for the chipload.

Pine probably would be fine but remember it does like to cup as it dries out. Try one and see how it goes. I hope this helps you in some way and I am sure others will give their advice as well.

I took a look at that, Thanks!
If I have this correct, running 12K rpm, with 2 cutting edges, and a chip load of .016; would give me a feed rate of 384 ipm? Do you agree with that? Also, if that is correct...my feed rate was way to slow at 100 ipm. I have never run anything near that fast, that is why I am just double checking!
Thanks again for the input!
Mark

Also, it states 1x D, so with a 1/2" bit, I should be taking 1/2" per pass?

It would appear you had a 0.004" chipload with the speeds you were running. I would start with 0.08 - 0.012" and go from there. Try 10k RPM and 180IPM. That would be a starting point. Depth of cut would depend on the tool but I would start with no more than 1/2 of the diameter while testing. This is an assumption but I think most Mechmates are not run that fast and doubt if it would render a good finish cut. I have run 240IPM before but I am selective on the speed based on the material and bit.

Remember these are calculations and will have to be run adjusted. They normally say with the calculated to start with 70% for the feed. So if your feed is to be for example 200IPM then either start with the g code set to 140IPM or set your feedrate override to 70% before starting. If you have a good bit you trust, you could start with full pass depth of 1/2". But don't jump in whole hog, test and inspect, modify and test, modify and test. Once you see the finish deteriorate or the bit too hot then back off to the previous setting.

Thanks Pete, that was very helpful. I am over 200 ipm with good results and making chips instead of powder :o

I appreciate your feedback!
Mark

Well my bit is getting hot after 15 mins of cutting. My router will only go down to 10K, so is my only other option to keep raising the feed rate? If so, than is this an example of where a spindle is better than a router (being able to get lower RPM's)?
Mark

You could use air assist cooling but only if you have adequate dust collection. It does take a lot of air just a trickle or break up your continuous run to give a little cool down time.

ok, I can break up the number of parts into smaller runs and get through this job. Do you know, if I am correct about my logic on the spindle vs. router? Wouldn't mind "to have to" get a spindle :)
Thanks
Mark

You could run the spindle at 8000 or you could go to a single edge tool

I am hearing that I should buy a nice new spindle for #119....I'm gonna tell my wife you said so!
Again, really appreciate your help, Pete.
Thanks
Mark

I would opt for a different tool first but if I must be the reason I can be that also.

Even with the spindle I would go with a single flute cutter.
I would guess that some of that heat is generated by the router being run under less rpm/power, at least that is what I saw with my router when trying run in the lower speed range. A spindel will have no issues with lower speeds as long as you maintain the recommended speeds set by the manufacturer (8k min.)

Thanks Steve.
I have ordered some carbide single edge,and will give that a try. I dulled what I was using, I think I was ruining the plunge rate to slow. I was goning to post and ask, when setting the feed rate, is the plunge set the same?
Mark

<<is the plunge set the same?>>
I use a half speed on the plunge

I normally ramp in and rarely plunge as the bearings are not really set for an axial load but rather for a radial load. If you do plunge and do not know how the bit will behave start at 15 to 30 and listen to the process. If it is too aggressive, you will hear it. If not, you can increase it.

Thanks, I will do some experimenting on plunge rates and ramping.
But that gives me a starting point.
Thanks again
Mark