back to the ol drawing board....

will that work if the text is raised from the bottom of the pocket?

Yes - it "CAN" work that way. I do it all the time.

If you are using Vectric Cut2D you can select a pocket toolpath and include a larger clearance tool.

When selecting the vectors you will select the boundary of the pocket and also the text.

Calculate

In the preview window - you will have two toolpaths. One for the larger tool and one for the smaller tool.

Preview each toolpath and you will clearly see what it is doing.

Get you feedrate MUCK much higher. The 10 IPM is bad. OK to start the toolpath just to be sure the tool is in the correct place, but then increase it rather quickly. You should be minimum 40 IPM - but really - up at 90

Leo Voisine said:

... Feedrate wise - you should be 60 to 120 IPM --- 10 or 20 is WAY too slow - you are burning the bit. ...

Click to expand...

You need to consider the type of machine before making this kind of statement. These are good machines but not as beefy as yours. The Inventables recommended feed rate for MDF is a maximum of 40ipm. I have made many cuts in MDF using 2- and 1-flute 1/8" bits at feeds ranging from 10 to 30ipm with no burning. Making the cuts deeper and faster does burn the bit.

As I only have the one size bit, it had to be done this way. I'll be getting larger bits in about a week or so, then I can go a little faster. Nice thing to know for the future.

today's score: 3-4-2. three successes (2 small, and 1 large gear), 4 fails (3 plaques, 1 photo engraving), and 2 snapped bits. such a day on the ol learning curve....

Dan Noren said:

... I'll be getting larger bits in about a week or so, then I can go a little faster. ...

Click to expand...

That depends. For hogging the background of a plaque, I've used a 1/4" straight bit; next was a 1/8" ball end for the rest of the carving. For a couple of carvings, I had to use a 1/16" end mill to keep the inside of text as sharp as possible.

Leo has reminded us several times about the balance between material, bit size, spindle speed and feed rate. At first, I used a couple of different 1/4" bits, straight and spiral upcut, because I thought that made sense for faster cutting. In reality, I've found that using the correct 1/8" bit reduces loading and has allowed me to increase my feed rate.

leo, finally figured out how to do the tool paths you mentioned. cut2d has a feature called pocket allowance. not sure what it did, so i gave it a try. sure enough, in the preview it cleared out the waste, leaving a balloon around the text areas. i started it with .2 inch, then .1 inch with a 1/4 inch bit, followed up with a 1/8 inch bit for the cleanup. learning something new every day. now the learning curve is down to 98.987 degrees from 99.25....

Bill Sorry - yes you are correct - all machines have limitations - you need to work within the limitations of the machine.

Actually, my machine is about 18 years old and not all that capable as the new machines are. The new machines are capable of 300-600 IPM. I was thinking your machine would be capable of at least 200. If your machine can only cut at 40, then that is what you need to work with. Sorry for assuming wrongly what your machine can do.

I am getting a bit nervous about posting responses because I feel that I am irritating you and perhaps others as well.

I am not the most diplomatic person, and I am just trying to be helpful.

There is a calculated way to determine the correct feedrate for a given RPM and material and additional conditions. I have a spreadsheet calculator to help in that, but at the moment I cannot find it. When I do find it if you like I will post it. I did post it once before but the threads get lost in the shuffle.

-------------------------------

Dan - I was not talking about pocket allowance. What that does is to leave a certain amount of material in the pocket to that you can go back with another tool afterwards. That is SIMILAR - but not the same.



In the pocketing toolpath in Cut2D Desktop - look for the check box in the picture above. Check the box. That will allow you to select a larger tool from the tool library. You calculate that - and it will automatically create 2 separate toolpaths.



This is the calculated toolpaths. One is the larger tool to pocket out most of the material, the other is a smaller tool to fit into the areas that the larger tool cannot fit into.

The larger tool will cut the entire area - the second smaller tool will only cut the places where the larger tool cannot fit into.

When you select the vector lines you will select both the outer line for the pocket and also the text. That is what I did here.

Leo Voisine said:

... I am getting a bit nervous about posting responses because I feel that I am irritating you and perhaps others as well.

I am not the most diplomatic person, and I am just trying to be helpful. ...

Click to expand...

Leo, you don't irritate me anymore than I irritate myself! We're good. We all understand your excitement and knowledge about CNC machines. I've learned a ton from your posts.

I never assumed the machines such as I purchased were capable of commercial production. In some situations, they might be capable of much higher feed rates than we've discussed so far, but I'm being conservative so far. If one takes the feed rates Inventables shows in its Easel software, they range from 5ipm at 0.003"/pass for aluminum to 40ipm at 0.063"/pass for MDF; both assume a 1/8" bit. The only problem with their assumptions is they don't give the number of flutes on the 1/8" bit. Oh, well, there are other resources.

Bill,

OK,

I just found my chipload calculator. This is one that I am making myself. I am trying to make it a comprehensive calculator to include many materials and additional information I can muster.

Problem is - there are far too many sources of information and none of them are in full agreement. Reason is - this is not an exact science. It's close, but not exact. I just finished a cut in hard maple with a 1/4" 2 flute end mill with a 1/4 depth of cut at 200 IPM & 18000 RPM. That comes out to about .212 chipload. Based on my chart the recommended chipload is .020 and calculates a feedrate of 18 IPM.

CHIPLOAD - IS by far the most important variable to try to achieve.

The increased chipload helps to move the heat out of the cut on the chip and off of the tool.

When I first started cutting wood on my CNC I was thinking metals. I have been cutting metals for 40 years. Cutting wood is a bit different. Some concepts are similar, but wood is a different material. My first cutters are black, because I heated them to the point where I could not touch them. My recent cutting - yesterday - was done with a chipload of up to 200 IPM. At the end of the cutting I could touch the cutter. It war warm but by no means hot.

This Chipload Calculator is a work in progress. It works I use it. It is on the SUPER CONSERVATIVE side. I am sure as I develop it more - it will move from the super conservative to a bit more robust.
I strongly suggest NOT staying super conservative.

This is an Excel spreadsheet - if you need a different format - I can try to convert it.

View attachment Chip Load Calculator.xlsx

i see what you mean leo, and when i have larger bits for clearing, that will be used.

I know a guy that used to buy 2 bits per job he would increase the feed rate until he broke the fist bit then backed off feed rate installed the new bit and cut all day........

Leo, a comment on your calculator: I've cut more MDF than anything else, some as practice and some for finished product like table saw zero clearance inserts. After much trial, error and gnashing of teeth, I get clean cuts at 20ipm with a 1/8" 2-flute end mill. During all of my testing phases, using a 4-flute end mill caused a lot of burning. Your chart indicates I should be able to double my feed rate if I double the number of flutes. That's not my experience on any of the materials I've worked with from MDF, pine, cherry, maple, or hdpe. As an example, until I reduced to a one flute end mill, I was melting hdpe rather than cutting it.

that's pretty much what my friend dale had to say, 4 flutes generate more heat than 2 flutes. as to melting hdpe, you can put me on that list too, and i was using a 2 flute bit.

I would add that 8 flutes could calculate the feedrate to be faster - or 20 flutes even moreso.

The calculator does not account for unreasonable numbers - it is not a flaw in the calculation. In metals a 4 flute cutter would be very reasonable, but the chipload would be much lower.

When cutting wood, plastics, aluminum - the chipload is higher. By nature of the higher chipload, the gullet in the flutes needs to be larger to allow the chips to evacuate the tool. Using a 4 flute cutter in wood does not allow the chips to evacuate.

Using a 4 flute 1/8 end mill in MDF is absolutely a bad choice.

So - it's not a flaw in the calculator. It's all about using the correct cutter for the job.

In wood - a maximum of 3 flutes - on 1/4 to about 3/4 inch cutter.

Onsurd and others have single flute cutters.

BTW - did you calculate your feedrate based on what is in my spreadsheet just to see what you get? Around 20 IPM?

Dan Noren said:

that's pretty much what my friend dale had to say, 4 flutes generate more heat than 2 flutes. as to melting hdpe, you can put me on that list too, and i was using a 2 flute bit.

Click to expand...

Ayyup!!! Two flutes were better than 4 but I got the best cuts on those spindle brackets with a 1-flute 1/8" end mill. If I followed the charts I've seen elsewhere, I'd be burning or melting things like crazy. It appears to this novice that the charts I've seen are created by someone doing metalworking and assuming similar results should be true for wood and plastic.

Leo Voisine said:

... did you calculate your feedrate based on what is in my spreadsheet just to see what you get? Around 20 IPM?

Click to expand...

If I use your spreadsheet to calculate feed rate for hdpe, I get 20ipm using a 4-flute 1/8" end mill. If I actually try to use a 4-flute bit, the hdpe melts. I get good cuts using a 1-flute 1/8" end mill at 20ipm, but your sheet says I should use 5ipm. It's almost like your spreadsheet (and others I've seen) is backwards for non-metallic materials.

Bill,

You are correct - my calculation was in error.

I fixed the calculation - it is correct now.

As far as metals calculations or wood calculations or plastics - it does not matter - the formula to calculate IPM based on chipload is the same in any case. It is just math.

I don't think you will agree with the calculator, but none-the-less this is what it is.

I'm not going to repost it, because the feedrate for MDF with a .005 chipload and a single flute cutter is 90 IPM at 18,000 RPM. If you run your spindle at 4,000 RPM, 20 IPM will be a good number.

I do thank you for challenging my calculations - made me go back and look.


BTW - Why do you keep saying 4 flute? There is nothing in my spreadsheet that recommends a 4 flute cutter.

Leo Voisine said:

... BTW - Why do you keep saying 4 flute? There is nothing in my spreadsheet that recommends a 4 flute cutter.

Click to expand...

Your spreadsheet doesn't make any recommendation on flute count, nor does it limit the entry one can make in the flute field. The same is true of all of the online chip load calculators I've checked so far. I was simply using four flutes as an example of what might not work for all situations. One thing I haven't seen factored on the spreadsheets I've seen is depth of cut, which can make a big difference in feed rate.