Good bit for 3D work

[itamarj]

Hey guys,
I'm doing some 3d work lately that is pretty deep (around 3"-4" thick).
So far I was using the 1/8" tapered ball nose that came with the starter kit and it did a good job. but I think I should get something longer. I do have a 6" long 1/4" ball nose, but I wasn't sure how detail i'm going to use.
Do anyone know where I can get 1/8" that is 4"-6" long?
Or what do you think about 1/8" vs. 1/4" when it comes to 3d?
I read here in one of the thread that actually 1/4" will give better result, but I find it hard to believe.
Anyways, would love to hear your thought!
David

[Brady Watson]

David,
This is a difficult question to answer. No diameter bit is 'better' than any other. It boils down to how much detail needs to be picked up from a given diameter ball end tool.

You will most likely not find an off the shelf 1/8" bit over 4" overall length OR a 1/4" over 4 or 5" OAL. The bit simply has too much flex and deflection to be useful at that length. If you do, they will be very expensive & only be marginally useful in low density foam.

The best way to answer this question would be for you to use PartWorks3D or Aspire & run a cut preview using different diameter tools to see the result of different diameters.

Also - You should ALWAYS do a 3D roughing toolpath with a straight or spiral bit BEFORE you run your 3D finishing toolpath. This gives a better finish, drastically increases tool life.

-B

[dlcw]

David,

When doing large carvings, I do my rough path with a 1/2" ballnose. This removes a LOT of material very quickly. I then come back and use a 1/8" ballnose for the finish path. For small carvings I use a 1/4" ballnose for roughing and a 1/8" for finishing.

These combinations have always worked for me very well. The deepest I've carved is about 2", not the depths you're talking about.

[itamarj]

Thank you guys for your replay!
I learn by breaking my bit, that roughing is an essential part of the milling work, and I shouldn't skip it. At my first jobs I thought it will take more time and effort to change bit but now I notice that the finish wasn't perfect and i broke several bits.

Brandy, where can I find 4" long 1/8" ball nose? I looked through many website and could not find it anywhere.

[ssflyer]

David,

Something you might want to consider is slicing your model. That way you avoid the many issues with a really long bit, and works well.

Ron

[itamarj]

Hey Ron,
I was thinking to do that, but since I'm milling wood, and it's a delicate piece I'm not sure how well i'll be able to attach the two pieces together.
Also, I will have to surface the table and the wood itself to get an good finish. It's a lot of work, but that definitely a way to avoid using a long bit...

[itamarj]

I wanted to share my results, and hear some feedback about the work.
These are two reliefs that I just made. The first one is 1.5" thick and about 24"x14" and the second one is 3" thick.
With the second relief I worked with a dremel and added a lot of details in the undercuts and many other places (hands faces ect.)
I used 1/2" bit for the roughing and 1/8" taper bit for the finishing.
I have several question that came from this job:

1. The models are much more detailed than the result, maybe I can use a smaller bit after the 1/8" to get more details. Which bit would you recommend? should I use a 1/16" ball nose or a different engraving bit.

2. The second relief posed a problem because it was deep. I was concerned that my basic 1/8" taper ball nose is not long enough and the collet will hit parts of the relief while trying to reach into the lowest point. Luckily, it went well, but I was looking for a longer 1/8" bit and could not find any. I bought a 4-1/5" 1/8" bit from MSC (http://metalworking.mscdirect.com/CGI/NNSRIT?PMPXNO=4403719) but it's for 1/2" collet and I am not sure if the 3 degree angle will work well with this kind of job (3D milling). What do you think?

3. I saw that there are tool extenders (http://www.onsrud.com/xDoc/Extension) out there, but they are pretty expensive ($170 and up). Does anyone have experience with that? is that a good way to solve it?

4. This is very basic question, where can I find 1/8" collet for my Porter Cable router? Should I buy one of those Sleeve adapters to convert 1/4" collet to 1/8" bit (http://www.cadcamcadcam.com/sleeve-adaptor14to316-1-1.aspx)?

Many thanks for all your help guys!

http://www.talkshopbot.com/forum/picture.php?albumid=20&pictureid=114

http://www.talkshopbot.com/forum/picture.php?albumid=20&pictureid=113

[Brady Watson]

You need a stubby collet chuck for your PC router. It will let you use 1/8" and smaller bits without adding runout like the cheap sleeve reducers. I did a write up on this in the ShopBot web column area on the SB main site.

The tapered tools are expensive, but very robust. A popular bit is a 1/4" shank, 2.5" CL, 4" OAL 1.5 deg taper. They are not cheap, but they work well, are very forgiving and last a long time. You don't want to go too much deeper on an 1/8" tool since deflection becomes a major issue.

A picture is worth a thousand words. Post up what you are doing/have done...the comments and suggestions you receive will be worth much more to you.

-B

[itamarj]

Brandy,
Thank you so much for your reply. Your post on stubby collet chuck (http://www.shopbotblog.com/index.php/2006/01/just-a-little-bit/) was exactly what I was looking for. It hit two birds with one stone - both extends the bit and also allows different size shank tools. Perfect!!

I posted the pictures of my work through Talkshopbot forum album, but I guess they didn't got approved yet. Here they are again:

pic 1 (http://img217.imageshack.us/img217/8500/photo1ct.jpg)
pic 2 (http://img571.imageshack.us/img571/1492/photo2xq.jpg)

What kind of bit would you recommend for getting the little details on the relief (for the face and hands ect.)? would 1/16" ball nose do the job, or should I better go with an engraving bit?

Thanks again!

[dana_swift]

Did you do the 3D artwork for the carvings? That looks like you are doing very well for just getting started-

Congratulations and well done!

D

[Brady Watson]

Glad it worked out. My name is Brady...not BraNdy, by the way...

A 1/16" ball would clean things up considerably, but realize that the run time will be twice as long as the 1/8" pass provided the stepover percentage and speeds are the same.

It is difficult to find a 1/16" ball over .375 or .500" LOC. .375" is a SXL and .500 is a special.

-B

[itamarj]

Sorry Brady for messing with your name, English is not my first language, so sometime catch names wrong...

I was thinking to run the 1/16" not on the whole relief, just to add some detail ( I remember ArtCam have this function). Do you think a V-carve bit will be more suitable for that?

Thanks Dana :-)
I've been doing 3D work for more than 8 years now, but have the shopbot for only a year...

[Brady Watson]

David,
You can go over the whole relief with the 1/16", but make sure you set the stepdown on your roughing toolpath to a small number, like .0625" or something. This will take a long time to machine, BUT it will more closely follow the relief when you machine it - and it will drastically reduce bit breakage on the 1/16.

You also have to be careful about collet collision - which you are already aware of.

You most certainly want the ball end tool...no V bits.

Rest machining in ArtCAM leaves much to be desired. I prefer to create outline vectors that cover only the areas I want the 1/16 to go into - and where it must go for details essential to the carving.

I'm sending you a PM - check it.

-B

[itamarj]

Brady,
I just want to make sure that I understand you.
You think I should rough it out first (let's say with 1/4") and then go over the whole thing with 1/16" bit? so skip the 1/8" pass?

My initial though was to rough it, and then relief it with 1/8" and at the end, just adding details on certain places with the 1/16".

I though that this way, I don't need to care much about LOC of the 1/16" at all, since I'm just only adding some small details. I mostly want to add definition to the figures - (where limbs are intersect between two figure, or face features ect.). That's why I thought about v-carve or engraving cutters.

What do you think?

I tested out the rest machine in ArtCam with 60 v-carve and it looks like it was building toolpath in the right places, although i couldn't figure out the how to save the simulation results so I couldn't see a good comparison between the two.

[Brady Watson]

Yes - if your design is 'loose' enough to rough with a 1/4" - then yes, skip the 1/8" and go over the entire design with a 1/16". You just don't want the 1/4" to leave too much meat on there for the 1/16 to take down. The small stepdown when roughing is very important...not many people get this.

Rest machining in ArtCAM stinks...It often gouges and does stupid moves. I prefer not to use it. I've used ArtCAM since v5. I prefer to be patient, rough out (even with an 1/8" ball at 20-25%) and then just let the machine work with the 1/16 until complete. This will result in the best finish possible. I've been machining reliefs for the past 10 yrs....I never use a v-bit for finishing.

Of course, some discretion is in order - as no two reliefs are alike, machine the same or are conducive to certain strategies. Don't be afraid to try out new things & do your own R&D. Try rest machining on scrap material - see if you like the results.

-B

[billp]

If you want to "see" the differences in multiple "rest machining" tool paths, just do a few "print screen" screen shots so you can then lay them out in any image viewing program for comparison. BE SURE you label EACH screen shot before dumping it however!!!!!
And if you REALLY want detail you can get bits SO small they make the 1/16" inch look like a phillips screwdriver tip.....Many sources in past threads on this Forum.

[itamarj]

Brady, great, I'll try do that.
When you you writing using a small step down, how small do you mean?
My 1/8" path was with 1.3" deep on each pass, which was almost the LOC of the taper bit. It still had to run twice, since the relief was about 2.5" deep. It took forever. I think something about 16 hours, with 3" per second speed. I never leave the cnc unwatched and I had to stop it between the run. I don't like to do that, since I feel every time i'm pausing the machine for long time, the Z is never the same.

I think I'll go with your advise and not use the rest machine. Maybe I'll run the 1/16" only on the figures and it will save a lot of time.

Bill, I didn't think about screen prints. Great idea.

Thanks guys, I feel that I'm learning a lot from this discussion. I really appreciate your help!

[Brady Watson]

David,
The stepdown distance you enter in for your roughing tool on the 3D roughing strategy toolpath regulates how closely the toolpath will follow the relief, while still leaving .02" of meat for the finishing pass.

For instance, you may have areas that are just too deep to machine with an 1/8 or 1/16" because you set the stepdown depth too coarse - let's say, .25" per pass, then .23" might be too much for those small bits to shave off. But, if you set your stepdown at .125", then the finishing tool will only shave off .105" which is more reasonable. (EG - stepdown set to .25" & we leave .02" of meat, then if the stepdown is .25, it is possible for ArtCAM to leave .22" on the relief - which might be too much for a small tool - .24 or less will be ignored by ArtCAM if stepdown is set to .25")

This is hard to put into words & varies from relief to relief...In some cases, it DOES make sense to do 1) A roughing pass with a 1/4" square bit 2) A rough finishing pass with an 1/8" ball @ 20-25% stepover - full depth & 3) a finishing pass with a 1/16" ball.

-B

[itamarj]

Hey Brady,
I waited to all the new bits and parts to get here, to see if i have more questions. Everything seems to be ok, and I'm very excited to work on my new piece this weekend!

I didn't fully understand your last message. I think I might be confused with three terms - stepdown, allowance and tolerance.

I thought that allowance is the "meat" that you want to leave on the material - i.e. the offset above the relief, while stepdown means the maximum cut depth of the tool in a single pass. Another term I'm not sure about is the Tolerance - which in artcam i believe use to determine how closely the toolpath will be to the actual relief.

Now - If I understand you right - you saying that in some case it will make sense to start with a 1/4" - and than do a finishing pass of 1/"8 and then 1/16" - which make sense to me. I not sure I understand the stepdown though - in the first 1/4" I'm leaving .2" meat for the 1/8". If i'll set the stepdown of the 1/8" at .125" it will create many many path. I.E. if the relief is 3" deep - the first pass will be 2.875 and then 2.75 and so on...
it can take days till the 1/8" will go through all the relief, no? and it will not make sense since most of the material has been removed by the 1/4".


I'm sure I'm missing something...

p.s.
should I also leave some meat for the 1/16"?

[Brady Watson]

Just make sure that your roughing pass doesn't leave too much material on the relief before machining with the 1/16" bit. Just because you set the allowance (meat) to be left on the roughing pass, doesn't mean that ONLY .02" will be left on the relief. It means that a minimum of .02 will be left, and a maximum of your tool stepdown distance specified for roughing pass minus (-) .02" = How much could be left for the 1/8" or 1/16" to take off.

So...If you tell the roughing toolpath to go .5" deep per pass, then it is entirely possible for .48" of material to be left on the model before finish machining. This is what I was cautioning you about.

You should always leave a little bit on for the finishing pass. Even if it is 0.01".

-B

[itamarj]

Hey Brady,
Thanks, now I got it!
I working on the relief right now, and I went with a 0.5 to do rough-roughing and I felt it too strong and because I went with the grains the wood cracks. I read now in other thread that people recommend to go against the grain with the roughing. What are your thoughts about it?

I then changed to 0.25, and I broke the bit too times, I went to fast. I have to say that I didn't have a lot of patience and I learned my lesson. :)
The path had 0.2 allowance, and because the Z was off a bit few times, I wish I would have left more...

So with the 1/8" I went by the books (almost) and run it at .35" stepdown, 10% stepover and speed of about 1 ips. what do you think about that? (I'm using Walnut)
Is there a good table or source for those parameters?

I feel that the low stepdown creates a lot of unnecessary toolpath - where the bit travel over and over the relief in order to get to the border, or just "clearing" area that have been cleared by the roughing pass. I wish artcam would create a smarter path. Should I go back to use Partworks 3D?
What is the best tool to create 3D reliefs toolpath?


My last question is about leaving the machine to work on it's on. I remember that I've been to a bootcamp and when the subject came up people were concerned with fire. At my Grad school, we use to run a small CNC overnight all the time. A friend of mine also told me that they have a large CNC at school and they leave it to work unattended. Machine a detail relief I feel can take more than 40 hours of work, and it can become significant in my progress. What do you think about it?

Well for the meantime, I installed Icam application on my iphone (only $5), and have a webcam installed near the machine, so I can see the machine running on my phone or on a web browser. Now I feel a little bit safe to get out of the shop for 5 min. can get a snack :)

[jimmya]

I think if you use a .35 stepdown with an 1/8" bit in walnut, the bit will break for sure. Or did you mean .035?

Jimmy

[Brady Watson]

I read now in other thread that people recommend to go against the grain with the roughing. What are your thoughts about it?

It depends on the wood itself. A raster strategy is usually fine unless the wood is excessively dry. Use 40% stepover for roughing. With hardwoods you need to slow things down. If you have an extra deep relief, with an extra long bit, you MUST slow things down & limit the move speed to keep from breaking the bit in hardwood.



So with the 1/8" I went by the books (almost) and run it at .35" stepdown, 10% stepover and speed of about 1 ips. what do you think about that? (I'm using Walnut) Is there a good table or source for those parameters?

If you run a proper roughing pass, then you should have no problem moving 2,1 or 3,2 on the finishing pass. Stepdown doesn't matter in ArtCAM or PW3D, unless you tell it to machine the relief in multiple passes. This is a waste of time. Rough out & machine the relief full depth. This is where you have to anticipate collet collisions etc.

If you intend on doing some hand carving, scraping and sanding on the relief, then a 20% stepover will get you pretty close in 1/2 the time as a 10% stepover. This is the trade off....If you want a relief that needs minor touch ups, then run 8-12% SO. If you don't mind sanding etc & just want to rough out and get 'close', then a 15-20% is fine. Run tests in software preview of toolpath and scrap material to see the difference for yourself.



I feel that the low stepdown creates a lot of unnecessary toolpath - where the bit travel over and over the relief in order to get to the border, or just "clearing" area that have been cleared by the roughing pass. I wish artcam would create a smarter path. Should I go back to use Partworks 3D?
What is the best tool to create 3D reliefs toolpath?

The finishing pass should always shave off a little material in the Z. If you are talking about the toolpath machining outside of the actual relief, cutting flat ambient area - then the toolpath can easily be restricted using a vector outline of the area that you want to machine. Draw a 2D vector outline and (in ArtCAM) choose the 'selected vector' in the 3D toolpath. The 3D toolpath will restrict the tool to that vector boundary. PW3D will also do this by choosing the 'Use Model Silhouette' option on the material setup page.

The results between ArtCAM and PW3D are identical for most reliefs. It's only when you leverage some of the advanced toolpath options in ArtCAM that you may see a difference in very specific situations - such as machining a dome. For what you are doing, it is a matter of choice. Either will produce good results.



My last question is about leaving the machine to work on it's on. I remember that I've been to a bootcamp and when the subject came up people were concerned with fire.... What do you think about it?

I think that this is entirely up to you. I will not advise anyone on whether to do this or not. I will say that there is always a danger of starting a fire with an unattended machine. There is always the potential for the power to go out, the machine to do exactly what you told it to do - not what you thought it would do, and other hiccups that you just can't plan for. Only after I ran my machine for several years & felt I had the computer, communication and my own programming skills finely tuned, did I consider leaving the machine unattended.

I would focus on optimizing your toolpaths and getting those finishing times down so that you don't have to leave the machine unattended.

-B

[itamarj]

Hey Brady,
Thanks, things are much clearer now, and I start working on the new relief.
I rough it using 1/4" and 1/8" and now I'm finishing it using 1/16" ball nose bit.
I did use several path with stepdown of 0.4" since the length of cut of my bit is .5 and I was concern that in many places I'll have a problem if I'll run it in one path.

But I still predict some problem. The bit is 1/16" but the shank diameter is 1/8", the overall length is 2.5" and the length of cut is .5". Now, in area where the relief is very steep it might create a problem. Artcam will create a path thinking that the bit is 1/16" but when the bit will go deeper then the length of cut the actual bit is 1/8". So i'm not sure what going to happen, it might push the bit and offset the whole coordination.

The depth of my relief is around 2.7" and the maximum LOC that i was able to find was 0.95. Another problem is the overall length. I using the stubby collet and it's a huge help, but again the maximum OAL I was able to find is 3, and it's still a problem (specially since it's 1/8" collet bit).
Do you have any suggestion of how to solve this?

Btw - I were right about the amount of allowance that left after the rough pass - it's much thicker than what I asked Artcam to do. Thank you for this tip!
Here is an image of the work in progress, hope it will help...
http://img59.imageshack.us/img59/9059/photo4lm.jpg