Bit Degrees & number of flutes?

[applik]

Ok, you seasoned veterans. This is beyond me so I need it put in easy to understand terms. I'm carving 3D (relief) 1/4 to 1/2 deep into flat chunks of wood. So far I've used a 1 1/2 degree two flute tapered end mill and a 3 degree two flute end mill. Testing the same file with both bits, the 3 degree came out smoother. Should it be this way? I can also order a 5 or 7 degree and anything from 2 to 4 flutes on the various bits. What does the degree have to do with it? Should I order bits with more flutes also? I'm not even sure I'm using the right speeds n such, but I did some searches and came up with speed 1.5 ips/ plunge .5/ safe Z .2/ Mlkw router 15,000/ stepover .008. Does that sound about right? I like not having much cleanup to do on the carving even if it does take longer. Could I speed it up a little without breaking anything? The tips you guys gave me about rounding over the edges then cutting worked great! I've attached a pic of the two plaques we've carved and they came out wonderful. One is oak and one is pine. Size: 31" long x 9" tall. Sold them both and have to make 6 more. Yahooo. We are officially in the carving business I think.
Thanks again for all your help,
Shari

4767

4768

[mikejohn]

Shari
I don't do this type of work, so can't help, but I have to say they look fantastic.
Well done!

..........Mike

[jseiler]

Can you be more specific about the bits? Size of cutting end, ballend or endmill, where purchased, etc. It might help give a better answer.

Its hard to tell how much cleanup you needed to do, but often on my small 3d stuff, I can get away with a scotchbrite pad or a soft foam sand sheet.

Often what I do is let something cut a while, see how it comes out, pause cutting, insert a move speed command (MS 1,.5 for example) to speed up or slow down. It really helps to keep a notebook.

By the way, these look great. Congratulations. How long was the total cutting time at what speed?

John

[zeykr]

Very Nice!

I'm guessing you are using a 1/8 bn endmill. I don't think the taper should affect the finish, but would change the slope of any vertical wall's in your cut if you have one. 2 flute is probably what you want at the speeds you can cut 3d. Others have more experience and may be able to tell you more, but on a stock prt I run a 1/8 taper at 2.5ips move, 2.5ips plunge, .008 to .01 stepover, and change ramping for 3d work using the vr command. I'm not at machine right now so can't tell you VR settings I use for 3D, but they are basically the recommendation that Chris from shopbot talked about at the kansas camp. The VR changes make the 3d cutting much more efficient, but you need to remember to set them back when going back to 2d. Chris or Bradley can probably fill in more details on ramping settings.

To clean up, a friend recommended the small brass brushes you find at the lumber yard or hobby stores - they do a good job of removing the frizzies that are sometimes left on end grain. You can rub pretty hard without damaging the detail of the carving.

[zeykr]

Were the 1 1/2 and 3 degree taper cuts in the same material - or did you use one for the oak and one for the pine? If each bit in a different wood, I would guess the difference in smoothness of the cut was more a function of the material than the taper of the bit.

[applik]

I ran the same files in the same wood (pine) with the two different bits. Both bits are 1/4 shank, 1/8" tapered ball nose endmills. Not sure what hubby ordered, Onsrud maybe? I'm not complaining about the cleanup. There pretty much is none. Maybe a light swoosh with a brush and it's ready to stain. The file was 4 hrs/5 min as I recall. I am keeping a notebook plus writing info on the test carvings for future reference til I get the hang of this.
I would definitely like to speed up the machine a little so I'll try the 2.5 ips. If you can remember what ramp value you changed to please let me know. I haven't tried changing settings yet, so they are still factory I guess. I'll go back and read the book more and email Shopbot.

I named my bot "BlueBelle". She is a very hard worker and we're looking forward to a long and profitable relationship. Hoping to make her a 4x8 pretty soon. Got lots of new stuff to get carving on this week, so back to work.

Thanks,
Shari

[Brady Watson]

Shari,
CHange your VR 'Slow Corner Speed' to 40 or 50 and your 'Minimum Distance to Check' to .08. You *should* be able to run at 5,5 with no problems just changing those 2 settings.

-B

[zeykr]

OOPS! Thought Brady and wrote Bradley above. Sorry Brady. I have foot in finger disease a lot ;-)

[mikejohn]

Shari, I did a quick calculation that, with a 0.008 stepover, if you were doing straight lines up and down it would take 2 hours to cover the area.
The other 2 hours in your case comes from the constant ramping. Changing you IPS isnt going to greatly reduce your time, because of constant ramping.
However, with 4 hours cutting I guess even 25% decrease would be great.


.........Mike

[applik]

Brady,

You mean 5 ips and 5" plunge? Oh my, I may have a nervous breakdown watching her go at that speed! But it does seem ultra slow at 1.5. So I'll give it a go. Do I need to change these settings back when I cut the plaque out?

Won't be able to try this until late this evening. I'm off to help at a quilt camp. ;)

Thanks for the input,
Shari

[Brady Watson]

Yes. 5IPS on both, WITH the VR changes mentioned. I would do the cut out pass at your 1.5 IPS. You only need to be biting your nails on the 1st pass...every pass after that will only be shaving off your stepover amount, and only the 1st pass buries the bit completely...So, more accurately, run your 1st or 2nd pass @ your 1.5 IPS, then hit the S-key, then I to insert and MS - Change your MS to 5,5 (and be sure that you have changed your VR values to the ones I mentioned before running at that speed)

If you are in doubt about any of these changes or your are simply afraid to try that speed, just throw a piece of foam on the table and cut that 1st. In more recent times I have cut 3D @ 8,8 with lots of ramping tweaks. You should be fine @ 5,5.

You may also want to try changing the 3D threshold value to 150 instead of 100.

BTW...all of these settings are for Alphas and NOT PRT standards. 4G settings are close, but not exactly the same as Alphas.

-B

[mikejohn]

Shari
If you do increase your speed from 1.5IPS to 5IPS, I would be interested to know what time reduction you get with your file.

................Mike

[zeykr]

Brady,
How should 4G settings be different?

[Brady Watson]

Since the unit values on the 4G are 1800 and the Alpha are around 1200, you need to shorten the ramps to around .2 all the way down the list. I've had the best luck with settings between .16 & .24 all the way down the line, but I haven't had much time to tinker with my 4G setup these past few days.

-B

[applik]

Brady,
I want to thank you for the settings. I trusted your judgement and just laid a board down to carve. Worked great. The time was 2hrs/56min and it came out smooth as silk. We may eventually work up to the 8,8 that Chris from SB suggested. Will wait til we get used to the 5,5 first. ;)
I checked the original file sheet and the carving time was 4hrs/53mins! That's a huge time savings with excellent carving results.

Thanks again for all the help. Bluebelle is working hard as I write. She is definitely a keeper.

Shari

[Brady Watson]

I love it when a plan comes together!

No problem on the VR settings...Your machine can cut faster than 5,5 but it is not such a bad idea to be conservative until YOU feel comfortable running at those speeds.

-B