3d with multiple roughing toolpath

This forum is for general discussion about Aspire
nassau
Posts: 3
Joined: Thu Oct 27, 2011 10:55 pm
Model of CNC Machine: blurry

3d with multiple roughing toolpath

Post by nassau »

Please help. i'm trying to make large 3d crests for a customer. the material is 3" thick and i would like to do a rough pass with a 1/2" bit, and then a rough pass with a 1/4" bit to get into the details a little better. Finally a finish pass with a 1/16" ball end.
anybody have a trick for that?

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

Yup, there are definitely some tricks to doing this sort of thing.

First off you need to figure out if you are going to need a gutter around the part to allow the collet with smaller finish bit to clear. I am working on one now that is about 2 inches deep, looks like this:
Capture.JPG
Notice that gutter around the outside. The way I do this to save time is create during the roughing tool pass rather than making a bunch of profile cuts. To do this I create a flat component a little bigger than the outer boundary of the model. If the material is two inches thick and I want the gutter 1 inch deep I make that component 1 inch thick and set it to Merge. Now when I run the roughing pass with the big honking end mill it will only run to that depth.

After that I use a .25 ball nose with about a 30% stepover leaving .06 on a roughing pass with that flat component turned off. That allows the tool to get into smaller areas. I set the depth of cut to more than the model thickness so it only makes one pass. That avoids a bunch of unnecessary air cutting time.

That gutter should be somewhat wider than one half of your collet diameter.

I leave .06 on that second roughing pass because I run the machine at 300-400 IPM and that can result in some tearout in the pine I typically cut. So I have found that leaving that much is not a problem for the small ball nose bits.

Scarey stuff when you watch the collet nut on your machine go below the top of the work surface.. . . .

Hope this helps!
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: 3d with multiple roughing toolpath

Post by adze_cnc »

Do you really need to use the 1/16" ball end bit for all the finishing? Can you use a larger ball end cutter and then use the "rest machining" technique (there is a tutorial video on the Vectric support site)?

For an extreme "gutter" see accompanying image. It needed to be that deep for the 6-inch OAL ball-end bit to get deep enough. (The material is 7 feet long and 5.5 inches thick.) The other side had a similar need for a gutter.

Steven
Attachments
extreme-gutter.jpg

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

adze_cnc wrote:Do you really need to use the 1/16" ball end bit for all the finishing? Can you use a larger ball end cutter and then use the "rest machining" technique (there is a tutorial video on the Vectric support site)?

For an extreme "gutter" see accompanying image. It needed to be that deep for the 6-inch OAL ball-end bit to get deep enough. (The material is 7 feet long and 5.5 inches thick.) The other side had a similar need for a gutter.

Steven
I have mixed feelings about "rest" machining. Just my opinion which along with about $3 will get me a cup of coffee. It is sort of fiddly. I think it works well on some models but others, not so much. And then one had better have an electronic touch off plate or the results can be less than optimum. That model I posted above is an example, it just does not lend itself to "rest" machining. Most of it could be cut decently with a larger ball nose than I am going to use, but I like to get the vertical corners as sharp as possible to get a decent shadow line.

I dunno, maybe I have to work with the "rest" machining technique more to see what I can get out of it.

I would speculate that with a crest there is going to be a lot of detail that needs to be sharp as possible.
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
adze_cnc
Vectric Wizard
Posts: 4325
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: 3d with multiple roughing toolpath

Post by adze_cnc »

I've never tried "rest machining" myself. If I need ultra-high detail I'll block out those area that need it and cut them with a small cutter and leave the rest of the area to a larger cutter.

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

adze_cnc wrote:I've never tried "rest machining" myself. If I need ultra-high detail I'll block out those area that need it and cut them with a small cutter and leave the rest of the area to a larger cutter.
Yup, seems a lot less fiddly that way if you were to ask me.

I think my big "trick" concerns using a "ghost" flat plane component to control the depth of the first roughing passes. Then I can set a .25 ball nose so that it can cut deeper than the stock with a smaller stepover to remove all the stuff the larger end mill missed to prevent surprises in deeper pocket areas.
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: 3d with multiple roughing toolpath

Post by IslaWW »

Ted...
When you say:
"I leave .06 on that second roughing pass because I run the machine at 300-400 IPM and that can result in some tearout in the pine I typically cut."
Do you have video you could post or link to? The reason I ask is that I have done a lot of video diagnosis of cutting feedrates and acceleration using Camtasia which allows me to use frame timing to get actual cutting speeds. So if you look in this video:
At the 2:35 mark, when going fully across the model, because of the accel/decel 3D requires, actual cutting speed was actually 173.33 ipm, vs. the set 240 ipm.

The math: 5.2" across the model at the surface (longest point) 1.8 seconds to make a pass (average of 4 passes) results in 2.88889 inches per second or 173.333 inches per minute.

If I set the feedrate to 360 ipm on XY & Z, the speed across that section does not decrease. If I increase the acceleration for all 3 axes, then I can achieve slightly faster speeds, but only single digit percentage and at a bit of a loss of "smooth". The limiting factors are the vector lengths and angles, and the ability of the machine to accelerate and maybe more important, maintain a set speed thru these hundreds of angular changes.

That video was shot using a WinCNC controller, and I have seen similar results using a Centroid controller, but I feel it is highly unlikly that any of the hobby controllers will get close to that type of performance. So my guess is that you may be setting yours at 3-400 ipm, but it is doubtfull that it is actually maintaining the set feedrate. My test was done on a higher capacity machine with servos and just under 2000 ipm/sec acceleration, it would be unlikely that anything with steppers could match it, even if run on WinCNC or Centroid control.

Here is one with the exact same machine, running the same parts, same feeds, same rapids, same RPM, just different controllers. It isnt even close
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

Hey Gary,

No, do not have a video.

Of course it is not going 300 IPM all the time, accel precludes that happening as we all know.

The issue with 3d work is that often the tool is moving across a fairly flat surface, at that time it is moving at the programmed feedrate. Then it has to start decelerating because of a more radical upward movement on the Z, once it has changed direction then it begins accelerating again. But because of the typically short Z moves it cannot reach the targeted speed and then another significant direction change. And so on and so forth. But you knew all that already.

Here are some examples of what happens for anyone reading this stuff:

From a dead standstill, acceleration in the control is set to 24in/sec 2.

What happens in the first .1 sec?

The machine moves .12 inch.
The machine is traveling at 144 IPM

So it is apparent that if a move is .24 long (do not forget it has to slow down at the same rate) it will peak at 144 IPM but the average speed will be quite a bit less than that.

If you want to play with these numbers here are two very useful links:

https://www.vcalc.com/wiki/vCalc/Distan ... celeration

and

https://www.calculatorsoup.com/calculat ... ty_a_t.php

Gary, your example is not telling the whole truth. If I program a large model with smooth curves (say 48 inches long) the actual speed will start to approach the programmed speed. There is no getting around the accel/decel but when it is a larger percentage of the total time spent moving then it has a much greater effect on the average speed.

You wrote:

"The limiting factors are the vector lengths and angles, and the ability of the machine to accelerate and maybe more important, maintain a set speed thru these hundreds of angular changes."

Well, yes and no. Of course vector lengths are a factor and angles. But small angular changes do not impact velocity to any great degree because the machine will start the next command before reaching the end point of the current command. Effectively rounding the corner. That thing that is called constant velocity, which really isn't but sort of is. Also the machine has a look ahead buffer which helps prevent the "control cycle loop time" from becoming the controlling factor of machine speed to a point.

A way more interesting test than a straight line across a 3d model is to program a circle. Set the feedrate to something very high, start with a 1 inch circle and log the reported velocity. Keep increasing the diameter and eventually the velocity will start reading programmed velocity. I have been meaning to run this test two ways. The first with a series of G3 moves, the second with a circle constructed of bezier nodes. I am thinking the result will be the same because the control creates a whole series of tiny little moves internally when executing a G3 command. Obviously the control generates those tiny moves for a bezier as well, otherwise a circle with 4 bezier nodes would come out looking like a square.

BTW, that circle test is a much better way of figuring out average speed than watching a video camera film. You can program as many G3's in a row as you want achieving a very long distance, but that distance only has one accel and one decel. You can run this test on XY, YZ and XZ. XZ and YZ if you have enough Z travel to allow a circle big enough to reach targeted feedrate.

And with some creative programming you can get the elapsed time without using a stopwatch.

One of the reasons I mention this stuff and why I enjoy conversations like this is because we constantly hear on this forum and others: "There is no point in programming a high feedrate if you are doing 3d work." That is just patently wrong. True, depending on the model the machine may never reach that programmed feed rate ever. But the point is to have it accelerating to the maximum feed possible on every move. Or at least to the maximum feed that produces a good surface and the machine still runs smoothly. The model I showed on another post of a hummingbird and some flowers is a good example. There are some drastic height changes but there are also large smoothly curved surfaces (the model is about 24 X 18 X 2) The machine easily achieves a 150 IPM programmed feed rate over the larger curved smooth areas.

So do I think the controller is lying to me when it says that it is running at 300 IPM over a large curved surface on a model? Nope. Do I think that a small intricately detailed model will even come close to running at 300 IPM? Definitely not.
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: 3d with multiple roughing toolpath

Post by IslaWW »

Ted...
Point 1:
You need to go back and check your math. Using your example 24 in per sec per second acceleration. 1440 in per minute per second. Lets also assume that accel is trapezoid rather than S curve. And lets also assume that there is a very low or ~zero deadstart setting. And lets also forget that that the first tenth or two are actually spent overcoming the magnetic torque "detent" of a stepper motor. So we make the accel a pure linear (linear, but angular) representation of speed over time. The theoretical velocity trap starts linear, but few if any motors can deliver that.

The example you give that shows 144 ipm and 0.12 inches should read 1.2" Ten times your stated distance to achieve 144 ipm.
The math: 24 ips^ (or 1440 ipm/sec) =accel. Distance covered in 1st second = 12" at avg. velocity of 12 ips or 720 ipm. Distance covered in 1/10th second = 1.2" at avg velocity of 72ipm. Velocity at end of 1st .12" segment would be 14.4 ipm


When I wrote:
The limiting factors are the vector lengths and angles, and the ability of the machine to accelerate and maybe more important, maintain a set speed thru these hundreds of angular changes.
That was the truth, the whole truth and was completely verified by your statement:
If I program a large model with smooth curves (say 48 inches long) the actual speed will start to approach the programmed speed. There is no getting around the accel/decel but when it is a larger percentage of the total time spent moving then it has a much greater effect on the average speed.
Point 2:
Machines with higher acceleration will cut the same given file is less time. Thats a given, but on one with a Z axis that is capable of mathing the XY in "normal 3D" feedrates and acceleration should cut faster in cases similar to your posted example which is what I was referring to. XZ or YZ angular changes should happen as fluidly as XY. The reality is that hobby controllers usually have no more than 3 velocity/acceration settings vs the 7 to 10 that higher end controllers have. These additional settings allow much smoother 3D type, i.e. short vector, angular cutting to occur much smoother at much higher feedrates. This allows machines that upgrade to Centroid or WinCNC controllers to cut the same files in 40-60% of the time the same machine took with its previous controller.

Point 3: Go back and do your homework on that bezier stuff. Its all incorrect. The controller will generate the segments for an arc with G2/3 moves, but beziers will always be executed by the CAM's post processor outputting the segments. Even if 4 beziers form a perfect circle.
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

Point 1:
You need to go back and check your math. Using your example 24 in per sec per second acceleration. 1440 in per minute per second. Lets also assume that accel is trapezoid rather than S curve. And lets also assume that there is a very low or ~zero deadstart setting. And lets also forget that that the first tenth or two are actually spent overcoming the magnetic torque "detent" of a stepper motor. So we make the accel a pure linear (linear, but angular) representation of speed over time. The theoretical velocity trap starts linear, but few if any motors can deliver that.

The example you give that shows 144 ipm and 0.12 inches should read 1.2" Ten times your stated distance to achieve 144 ipm.
The math: 24 ips^ (or 1440 ipm/sec) =accel. Distance covered in 1st second = 12" at avg. velocity of 12 ips or 720 ipm. Distance covered in 1/10th second = 1.2" at avg velocity of 72ipm. Velocity at end of 1st .12" segment would be 14.4 ipm


Sorry, no, you need to check your math:
c1.JPG
I have nothing to support this but I think a tenth of a second is an eternity when it comes to electricity overcoming a "magnetic torque detent".

When I wrote:
The limiting factors are the vector lengths and angles, and the ability of the machine to accelerate and maybe more important, maintain a set speed thru these hundreds of angular changes.
That was the truth, the whole truth and was completely verified by your statement:
If I program a large model with smooth curves (say 48 inches long) the actual speed will start to approach the programmed speed. There is no getting around the accel/decel but when it is a larger percentage of the total time spent moving then it has a much greater effect on the average speed.


What my point there was is that when using a fairly short distance the impact of the accel/decel is more pronounced than over a long distance. I think you would agree with that.

Point 2:
Machines with higher acceleration will cut the same given file is less time. Thats a given, but on one with a Z axis that is capable of mathing the XY in "normal 3D" feedrates and acceleration should cut faster in cases similar to your posted example which is what I was referring to. XZ or YZ angular changes should happen as fluidly as XY. The reality is that hobby controllers usually have no more than 3 velocity/acceration settings vs the 7 to 10 that higher end controllers have. These additional settings allow much smoother 3D type, i.e. short vector, angular cutting to occur much smoother at much higher feedrates. This allows machines that upgrade to Centroid or WinCNC controllers to cut the same files in 40-60% of the time the same machine took with its previous controller.


Of course machines capable of higher accels/decels will cut a job in less time, we agree. I am not arguing that a higher end control will not cut faster. However, I am not going to agree with your statement that those controls will cut "the same files in 40-60% of the time...". That number appears to be based on your empirical data cutting smaller 3d files as shown in your video. I think that 40%-60% is misleading as a normal reader would think that would encompass all sorts and sizes of 3d work. The obvious benefit of higher accelerations is more pronounced in highly detailed work, as the detail level drops so do the advantages. Let's put it this way, I don't think you would want to bet that the Centroid or WinCNC controllers would cut a large dome shape 40-60% faster.

Point 3: Go back and do your homework on that bezier stuff. Its all incorrect. The controller will generate the segments for an arc with G2/3 moves, but beziers will always be executed by the CAM's post processor outputting the segments. Even if 4 beziers form a perfect circle.

You sort of got me there, trust me, I know about bezier files. The problem is that I have worked on machine controls that process bezier files directly rather than via a post processor and I conflated a bit.
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: 3d with multiple roughing toolpath

Post by IslaWW »

Ted...
My bad on the velocity over time calcs. I forgot to square the time, I was doing this in my head (too late) with scratch paper and simply muffed it. I too enlisted the aid of an online calculator (after a coffee or two this morning) and agree with your numbers.

Back to the original point. You showed an example of a file, what I would call a "pretty typical Vectric Relief model", the type cut by a majority of "normal readers" as you refer to them. I am referring to that type of file. If you wish to interject an out of the box "large dome model", I would then propose that I should interject "using a machine not capable of 24"/sec^ acceleration", like most of the homebuilt, desk and tabletop that "normal readers" own.

Your example uses a vector length of .12 inch, which is much longer than curved vector "generated segments", maybe 10 times as long, maybe even 50 times. So in most cases the slowdown, which in your example of a .24" vector with accel & decal produced an average velocity of 72 ipm, would result in much longer run times than a vector length calculator would show.

What I was referring to in my original post is that for the vast majority of users 3-400 ipm is much too fast, and that even if set speeds and acceleration were set to your examples, that the majority of PC based or handheld controllers are not capable of outputting 3D code that fast and holding detail. I.E., the speed interpolation calcs and the transmission rates of the comm cable (parallel, USB, etc) are known to the developers and they have intentionally throttled back the speeds at which they will run.

This is evident most on 3D or your example of circular files. Many of these controllers are able to buffer and spool up G2/3 motion but choke a bit when given that same segmented code via a posted file. Seldom executing them at the programmed feedrate. Take a 3" Vectric generated circle, toolpath it 1/2" deep, 1/8" per pass and select "Spiral" ramping. Use 100 ipm for feedrate in XY and Z. This will give combination of segmented circular interpolated files that engage all 3 axes without causing any Z related feed slowdowns. This toolpath will generate 4 ramped down passes and one that is level at Z depth. Do they all cut at the same feedrate? Now resize to .001 larger in either X or Y, which converts to curves rather than arcs and retoolpath. One last test, if your controller has the capability, using the first example with arcs, use the new Vectric feature that enables Z depth change during G2/3 moves. In theory all should execute within 1 or 2% of the programmed feedrate, which is more than reasonable for that sized vector. Few budget controllers will.

I will stand by my 40-60% number, with the caveat that it applies to the factory controller setting of most OEM type machines, and if you care to video your example above being aircut, I will do the same with your file. I don't think that I would get as high of numbers when compared to a machine tuned by someone knowledgeable like yourself, but I am willing to bet that the difference will surprise you more than me.

Thanks for the problems and the fun, (and the corrections too) GC
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
BradyWatson
Vectric Craftsman
Posts: 136
Joined: Fri Jan 13, 2006 5:57 pm
Location: South Jersey, USA
Contact:

Re: 3d with multiple roughing toolpath

Post by BradyWatson »

Ted,
I'd like to see your CNC roughing at 300-400 IPM. Care to post a video? Pics? Specs? Sounds pretty amazing for a home built machine running on a 20 year old controller. I would genuinely like to see it Z level Roughing a 3D part at those speeds.

I've been feeding my family for 2 decades cutting 3D parts on CNC routers and there's just no way the bulk of materials can be roughed out that fast. HDU? Maybe. Maple? Forget it. Ain't happening. Pine? Doesn't really matter I guess - GIGO. I haven't commercially cut pine in ages. It's junk. But then again, I don't buy any materials from the local big box store - where many users buy their material exclusively - which is in lockstep with typical Vectric stuff on budget or homemade machines.

Ideal feed calculations mean next to nothing in the real world - when it comes to lightweight aluminum extrusion gantry tools that deflect, shake, rattle and roll when accel/decel is very aggressive. Few ever want to admit their machine is capable of flexing enough to telegraph into the cut/part - and even fewer observe or test for that prevalent 'feature' among light CNCs. When you stop and really inspect the finished parts, they tell the tale...Besides, few here ever cut anything 3D larger than about 12" square, either because that is the average sized part or their machine isn't a whole lot larger than that. 90% of things 3D cut fall within that footprint - even in a job shop. Is it possible to cut at 300-400 IPM roughing? Absolutely...but it isn't very common & people shouldn't be lead to believe that it is. On a large relatively smooth relief, it is possible to rough or finish at say 720,720 - but on the OP's relief? Most machines would be hard pressed to truly cut at 200,200.

I guess the exception I take with posting roughing speeds of 300-400 IPM over and over, post after post, is that it isn't reality. Because I am not a hobbiest and do this work for a living, I felt the need to comment. Many have machines that are open loop - not capable of accelerating up to anywhere near those speeds without losing steps. Furthermore many hobby controllers will run choppy or even slower at high feed settings (ShopBot comes to mind here) - so rather than be lazy about posting high speeds to every file, I try to educate people to set the proper speeds for the work to be done, by imagining in their mind's eye how fast a profile will cut when commanded at a given speed. Clearly you have a pretty good handle on CNC and others look up to you for answers...However, with that comes a responsibility for posting correct information with the caveat that nearly nobody will be able to rough at that speed on their CNC. For instance, you'd be hard pressed to do that on any of these popular machines: ShopBot, Shark, XCarve, OX, etc, which many here have. Plus, many only have spindles capable of 18k RPM or even worse, hand routers that bog under the slightest change in cutting load. Not to mention hysteresis in the 6-8mm wide, long belt driven machines many people use...

What I have always advised people do, is to start out at a conservative baseline speed, such as 100,60 and then adjust the feed and RPM accordingly because every machine is different, as are materials and tooling and of course, hold down effectiveness. This is essentially the 'art of CNC routing' and all part of properly learning this work. I teach others to use their powers of observation and to watch (and adjust) machine 'behavior' as it were, to give the best quality results, using best known methods consistent with this craft.
High Definition 3D Laser Scanning www.IBILD.com

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

BradyWatson wrote:Ted,
I'd like to see your CNC roughing at 300-400 IPM. Care to post a video? Pics? Specs? Sounds pretty amazing for a home built machine running on a 20 year old controller. I would genuinely like to see it Z level Roughing a 3D part at those speeds.
Sorry I do not have a video of it roughing at 300-400 IPM. But I do have a video of it roughing at 800 ipm and profiling at 550 IPM. The video quality is not that good since I just stood there with my camera in hand. I published that video over 5 years ago and have posted it here several times for those who like to call others liars.

https://www.youtube.com/watch?v=Pt8n43_YRjI&t=51s

Other than that, it is nice to know that you think pine is junk wood. It also helps to understand that you feel machines made out of aluminum extrusions are not capable of the feed rates people use on them every day. We are all just such a bunch of, of, well, AMATUERS!

You wrote:

" Clearly you have a pretty good handle on CNC and others look up to you for answers...However, with that comes a responsibility for posting correct information with the caveat that nearly nobody will be able to rough at that speed on their CNC."

No Mr. Watson, I do not have a "pretty good handle on CNC". I did not work in a cnc router shop for 20 years feeding my family. Instead I spent about 20 years of my 45 year career designing cnc machines, I spent the other 25 writing CAM software for industrial lasers. I definitely do not know it all, but I do know a Japanese guy that pretty much does know it all. In fact, I know more than one of those guys.

Well, tomorrow I am going to go out to my shop and remember to tell my machine that it cannot cut 6mm deep into pine with a 10mm end mill traveling at a piddly 300 IPM. But yanno? The darn thing will just do it anyway, and it won't even shake, rattle and roll. How about that? What is worse is that those crummy aluminum extrusions are sitting on a pile of big box pine! Oh, the horror!

Edit: I forgot to mention! Did you notice the hand router being used as a spindle in that video? WOW, huh? Every time I watch that video I am waiting for it to "bog down" under load as you state they do. What is with that? BTW, that is a .5 end mill cutting .25 deep. Just for a frame of reference for you.

A further edit: Cutting on a cnc machine is not a craft and it is certainly not an art. Designing models would be an art, cutting them with hand tools is definitely a craft. But electrons flying through a micro processors? Nah. I would call a well trained operator a skilled operator, but not an artisan or a craftsman.
"If you see a good fight, get in it." Dr. Vernon Johns

User avatar
IslaWW
Vectric Wizard
Posts: 1402
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: CNC Controller Upgrades
Location: Bergland, MI, USA

Re: 3d with multiple roughing toolpath

Post by IslaWW »

I have learned a long time ago, that once someone feels the need to post their qualifications, in lieu of real facts or data, I am outta here!

KA-BYE
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com

User avatar
TReischl
Vectric Wizard
Posts: 4584
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: 3d with multiple roughing toolpath

Post by TReischl »

Me too, Gary!
"If you see a good fight, get in it." Dr. Vernon Johns

Post Reply