Cutting a half pillar

[mikejohn]

This is an Autocad drawing of half a pillar.
2664
It is 50cm long 8cm wide and 4 cm thick in beech.
How easy will it be to cut this piece? (ShopBot will soon be here
)
Normally done on a lathe, but for construction purposes I would like to make it in 2 halfs.
Any hints would be appreciated.
......Mike

[paco]

I would suggest to continue doing it on the lathe and just cutting it in half on the table or band saw... to machine such a part with the PRT, you would wish to have an indexer... doing this in 3D would be a waste of time!?

[mrdovey]

Mike...

It's actually fairly easy to cut. You'll probably want to use a round nose bit and make longitudinal cuts. I've created a couple of web pages (http://www.iedu.com/DeSoto/CNC/) that may help somewhat. On my PRT-96 this would take between six and seven minutes using a 1" round nose and spacing the cuts at 2º.

...Morris

[paco]

Hello Morris!

...curious; which of your pages are you refering mike to?
I guess you are using an indexer right?! Or have you a lathe installed on your PRT? This late option, I wonder if it could be done and efficient...? ...once installed on the table, the lathe could be used to turn the blank and the PRT used to machine on it; doing only 2D (X&Z or X&Y) moves to follow a patern... hummm... a new project to think about...! sure this would'nt be like having an indexer; more like a standard lathe with an automatic patern "follower"...

[mrdovey]

Paco...

Nope. Imagine having a template for a lathe duplicator with a straight edge on one side and the part profile on the opposite side. If you imagine the flat side running along the bottom center of the blank, the profile describes a cutting profile. Now lift the profile edge a small angle - and you get a second cutting profile. Repeat until the template is lying flat on the other face - at which time you've cut that profile in the round. The very easiest case is a cylindrical section, which uses a straight profile edge. Here's a photo of a quarter-round blank cut into a 2"x4" piece of construction lumber:

2665
The web pages are those that deal with cove geometry; but a round is actually the same problem (with the curve inverted).

This is one of those things that's a lot easier to describe with pictures than words; but I hope I've helped some.

...Morris

[paco]

Okayyy...
Interesting! Well, I'll have to study your pages some more; math is as far as school is!! Seriously, this inspire me for some new projects... again! I'm now thinking about "special" mouldings; like the one you got just above... I'll be back if I find something good to use with a 2D design from a CAD...

[mrdovey]

Paco...

It's not as difficult as it would seem at first glance. It's been 45 years since I studied geometry, trig, and algebra in high school - but it's a bit like riding a bicycle - it comes back quickly.

CAD is a tool - something make work easier. It's even a /good/ tool (I used my CAD package to make the drawings on the web pages) - but CAD isn't the whole toolkit. The most powerful tool we have is the one that sits on our shoulders. (-8

I've been working on another web page showing how to make the calculations for cutting rounds (actually, it's done except for the drawings) and I'll add that to the CNC menu page when they're done. It takes me a day to put a set of drawings together and I just haven't been able to take the time.

...Morris

[beacon14]

If you are fluent on the lathe the technique for getting half-columns is to glue the blank up out of two halves, with a piece of paper glued between the halves. After turning, you can split the blank apart at the paper using a wide chisel and mallet.
A light pass over the jointer cleans up the paper residue.

[garyb]

As with Morris this is an easy cut.
We cut similar profiles all the time but on a larger scale from cedar beams, usually 8x4 x 48" and 96" in length. Depending on the amount of detail will take under an hour with 1/2" ball end.
Photos must be on the other computer but here is one of a rope pattern which is similar in cutting etc. Size is 6.25 x 48" cut with .25 ball end in about 35 mins or there abouts.


2666

[mrdovey]

Gary...

Oooo! Nice! (I like it.)

...Morris

[paul_a]

Hi Mike

On your drawing are the horizontal lines datum points forming a smooth curve to the profile or do they denote steps in the turning.

Paul

[paco]

Impressive Gary!
Is it from a 3D CAD/CAM?... or math?!
I have done some trying from a 2D curve design coordinates in a spreadsheet program but I'm not fluent enought in this kind of software to do what I want... still got to learn about thoses...

[fleinbach]

Great work guys!

Morris
What program do you use for cutting the coves and rounds. I presume from what you said you are more or less not using a 3D cut path but are running in 2D. I had thought of doing this but do not know of a fast way to make the cut file. I had thought of making a file for cove cutting with each cut line slightly higher or lower as nessacary to get the shape but this would take a while. Off course once the file was made I could cut a stock lenght but what I realy want to do is cut the cove in an arch or some other curved profile. I believe following the curve with the cut path would be faster and cleaner then the horizontal/vertical path of a 3D file. Does anyone know of any software that can do this?

[paco]

Something like that?

2667
I wish I could do that too but I think it's a step further than straight moulding/profile... I believe spreadsheet could of a use for this kind of purposes but one have to build/programed the sheet/grid numbers...

[fleinbach]

Paco, you got it, this is what I want to be able to do. I'm sure if I did a cross section of the profile I could plot the elivation of each path but this would take time. Not to mention creating multiple cut paths all with the proper depth setting. It seems there should be some software capable of doing this.

[mrdovey]

Frank...

I cheated. I wrote a program to do all of the calculating and to write the results as SBP commands. For the quarter round I did something like this (pseudo code):

MZ(safe_z);
MX(-tool_radius);
for (angle=0; angle<45; angle = angle + 2)
{y1 = radius * cos(90 + angle);
y2 = radius * cos(90 - angle);
z = radius * sin(90 + angle);
MY(y1);
MZ(z);
MX(part_length + tool_radius);
MY(y2);
MX(-tool_radius);}
MZ(safe_z);


If you can describe the arch in terms of a mathematical equation, then it should be relatively easy to make the cove follow that curve. I agree, I think it could be much cleaner (but I think I'd do a lot of "air cutting" first
)

...Morris

[paco]

Once you exported the curve design in DXF (from Insignia, I was able to set the tolerance to get a good points "sampling" of a 2D X & Y curve), you can convert it to coordinate points with FC command for DXF file (there might be other ways to get the coordinates from a DXF...?). Then, you got the curve sampling points in the X & Y and from there, you can easily work the grid/coordinate numbers in a spreadsheet... but from there, I did'nt figure how yet to make it write an entire file for a defined lenght project... or better, to follow a curve as you wish to do...
Do anybody know more than me about using spreadsheet to write files?

[paco]

I begin to think that spreadsheet would be limited to a few thousand lines of code...

[mrdovey]

Paco...

Aren't you making a hard problem out of an easy one? Once you have the cross section of the curve defined (as in your drawing above), you can cut parallel "contour lines" that follow the curve of the arch. In other words, you set the z-height at the start of each pass, and use x and y to follow the contour line...

...Morris

[paco]

Sure Morris...
I agree with what you wrote; I think alike but how to write the complete file from this? Need more explanation about all this... each pass would need to be "offset" to the previous...!?
Curious; which software and/or what reference code did you use to programed your calculation and auto-writing?

[mrdovey]

Paco...

I think you've got most of the idea. The problem is three-dimensional only in determining the z-height of each contour line. I think your preferred approach might be to extract that from a drawing file; and mine might be to define the cross-section in mathematical terms and calculate the z-value directly - but both approaches are workable and each offers its own advantages and disadvantages.

If we go with the drawing file approach, my CAD program (and I'm sure yours does too) allows me to produce a line parallel to another line displaced by a specified distance - and if the first line is curved, then so will be the parallel line.

The computational approach is slightly more complicated, but gets me to the same place.

Either way, cutting the "contour line" is a strictly two-dimensional task.

Software? I write my own in the C programming language. The pseudo-code example is (almost) good C code. I actually have written the MX(), MY(), and MZ() functions (subroutines) and all each does is output an SBP command to the output file. For example, "MZ(safe_z)" writes " MZ " followed by the value stored in the variable safe_z followed by a newline character. If I'd previously set "safe_z = 3;" the program would produce the line " MZ 3" at that point in the output file.

Most arches are [1] circular, [2] elliptical, or [3] ogee (visualize the Taj Mahal or the Kremlin). BTW, ogee curves are actually two tangent circular curves - something that I only learned recently. Anyway, it's easy to produce concentric circles and to produce the elliptical equivalent.

Does this help?

...Morris

[garyb]

Here's a 5 minute profile and tool pathing for Mike's project to show he can do it no problem on the bot.(sorry I didn't smooth out the drawing but you get the idea)
Tool path calulated with 1/2" ball nose, .04 stepover in 14 mins. Working off his supplied dimensions

2668

[paco]

The sampling points I got from my 2D curve are'nt spaced equaly if you look at 'em in a axis way... they are spaced equaly toward the lenght of the curve itself... what did was to draw a curve in 2D...

2669
...then export it in DXF format to then convert it to data coordinates... from this I got a SBP file in which you can read (this is only a sample of what I got)...
M2,0.0008,0.0390
M2,0.0048,0.0775
M2,0.0119,0.1155
M2,0.0219,0.1528
M2,0.0503,0.2247
M2,0.0888,0.2917
M2,0.1365,0.3528
...and so on... you can see that the first value is'nt spaced equaly... from this, I can use the Y value as a Z value for height defining... and I got a X that I can use as either a X or a Y value depending on which axis the lenght of a straight moulding could be machined. But since the second value (the one I would use as a Z) is spaced equaly on the lenght of the curve AND NOT from the lenght of an axis, I would'nt have a clue how to offset each pass from each other... what I figured to do is to use thoses two values as Y & Z and to produce a X that would go back and forth along the lenght of a straight lenght of a blank... but how to program to obtain a back and forth like...
0,0.0008,0.0390
10,0.0008,0.0390
10,0.0048,0.0775
0,0.0048,0.0775
0,0.0119,0.1155
10,0.0119,0.1155
10,0.0219,0.1528
0,0.0219,0.1528
0,0.0503,0.2247
10,0.0503,0.2247
10,0.0888,0.2917
0,0.0888,0.2917
0,0.1365,0.3528
10,0.1365,0.3528
...from the previous example? This seem to me even more complex if one think to do this on a curved moulding!?!?!?... Maybe I need more help!

[mrdovey]

Paco...

For the back-and-forth case, iIf you add an "END" line to your converted file, I think you can do something like this in an SBP program:

&safe_z = 3
&part_length = 10
&tool_radius = %(20)/2
&next_x = -&tool_radius

open "converted_file.sbp" for input as #1
MZ &safe_z
MX &next_x
&next_x = &part_length - &next_x
loop:
input #1 &op,&y,&z
if &op = "END" then goto done
MY &y
MZ &z
MX &next_x
&next_x = &part_length - &next_x
goto loop

done:
JZ &safe_z
close #1
:

...Morris

[paco]

THANKS! VERY INTERESTING!!! I'll give it a try thomorrow...

PS for other tester: SB3 (Window version) use %(23) as for the cutter value...

[mrdovey]

Paco...

Glad you like it (First one is always free. :-)

SBP programs are painfully slow - and don't provide much in the way of error detection or recovery. It's almost always better to use some other programming language to do this kind of job, then run the converted file.

My SBP programming reference is at the shop so you might want to take time to check my handling of reading the op and end of file detection. It's been a while since I've written and run code like this - /I/ wouldn't trust it. Please don't /you/ trust it.

%(20) --> %(23)? Argh! I think I just heard the sound of all of my old part programs breaking...
( BAD Gordon! )-8

...Morris

[paco]

Yeah well now you got my brain working like a CPU man! I try to relax and just can think of new uses for such programs...
I sure will cut some air first... but seem logic...
Where would you suggest to start from about learning other type of programming? I did some search but got about 000000000000000000 after the first digit as the results found for "code programming"!!!
Will I be able to sleep tonight!? 8-D

[mrdovey]

Paco...

There are a number of ways to get started; and no way for me to give /any/ answer without having all kinds of people jumping up and down yelling "Yabbut..."

My sugestion would be to learn C. It isn't the easiest - but it's available for free for just about every computer in the world - and it allows you to do just about everything that can be done on a computer.

I have a web page for beginners (http://www.iedu.com/c/) - originally pointed to by the sig I used when posting to comp.lang.c (news:comp.lang.c) - of links to a number of C resources. One of those resources is a list of books. The clc (comp.lang.c) newsgroup is frequented by some of the best C programmers in the world who enjoy helping people learn. If you decide to subscribe to clc, I'd suggest lurking (reading without posting) for at least a week or two; and saying that you've done that in your first post. You'd probably also gain standing with the group if you mentioned the articles you'd read from my list of resources - these guys best like helping people who show that they're willing to help themselves. There's also fr.comp.lang.c (news:fr.comp.lang.c) if you're a French speaker (I peeked at your profile.)

Another of the resources is a directory full of C code files that you can download to see how this particular C programmer approached a number of programming tasks.

Finally (as a resource of last resort!) you can e-mail me for help. This is an activity I've tried to avoid because most of the people that sent e-mails didn't really want help - they wanted me to write their code for them. If you e-mail, make sure you've read "How to Ask Smart Questions" from the resource link list.

I think you have a lot of exciting times ahead!

...Morris

[paco]

Thanks you very much for thoses informations Morris!....

...but I need to go to sleep!!!... and now with this I won't be able to!!!
Seriously: I will first read the articles you are refering me to... before my last post, I already found some stuff about C code saying pretty much the same as you...
Thanks again!

[mikejohn]

Gentlemen all, thanks.
To answers Pauls question, its a continuous smooth curve.
My ShopBot is on the way. but not yet in my possesion, so for me it all remains theory.
Morris says to make longitudinal cuts. I recognise that if I cut laterally then each cut is a simple semi-circle in z and x (or y), but with many, many jog moves. I posted this yesterday evening (my time) before attending a family 'occasion' and I'm going to need more than this first cup of coffee before any few remaining brain cells kick in.I think cutting longitudinally has a different profile from first to last cut. This definately sems the quickest cutting method (I need to cut maybe 600 in a year) but at the moment how to arrive at the cutting file from the dxf defeats me.
Garyb's rope profile is fantastic, I'd love to do this, but imagine trying to match up the rope when you join the 2 halfs together.Thanks as always
...........Mike

[paul_a]

Mike

The turning is easily programmed with the Artcam Pro Turn Wizard, if you do not have the programme please let me know I will create a file for you to test on your Shopbot when you get it.

To 3D machine this on a PRT will take some time and the finish will not be as good as a lathe, as your profile is a continuous smooth
curve why not automate the lathe with the Shopbot.

My thought is to mount cheap lathe between the 2 main C channels on the back end of the Shopbot, make up a metal bracket that would be mounted to the Y gantry to hold a chisel type cutter to align with the centre of the lathe. The turning would be made up as David Buchsbaum suggested with the corners removed on the saw. The programming is a simple 2D cutting file set to repeat the pass cut for the amount of wood removal.

I am building this setup at present, I do have a few thing to get right such as the switchable limit switches to stop the cutter crashing into the lathe....nasty

If you want turnings as impressive as Garyb you will need to go the 3D route.

Paul



2670

[paco]

Morris-
It work! (I guess I knew that!?)
Some of the program had to corrected/changed/modified to run properly but most of it was OK...
-You were right about the way it was reading the "&op" at the end of the "converted file"; since it is looking for three values, I had to end the converted file as END, ,
-There were a slight error in the INPUT #1; missing a first comma before the first variable value...
-I changed the MY &y and MZ &z to M3 %(1),&y,&z to get a smoother transition between each pass... was giving...

2671
...and know look like...

2672
...still depends on the purposes...
-Added a JH at the end...
-The &safe_z was, I believe, not very useful...

So here what it is now...

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

&part_length = 10 '---Define part lenght
&tool_radius = %(23)/2 '---Enter cutter diameter in VC
&next_x = -&tool_radius

OPEN "file_name.sbp" FOR INPUT AS #1 '---Enter your converted file name
MX &next_x
&next_x = &part_length - &next_x
LOOP:
INPUT #1 ,&op,&y,&z
IF &op = "END" THEN GOTO DONE
M3 %(1),&y,&z
MX &next_x
&next_x = &part_length - &next_x
GOTO LOOP

DONE:
CLOSE #1
JH

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

One must note that to get a part that will actualy be the corrected size, he most previously offset the curve in CAD to half of is tool diameter used...
Now lets try to follow a curve rather than a straight path...

[mrdovey]

Paco...

Nicely done! Before you do the curve, there's one more piece of this problem worth looking at...

If you use the surface of the part as your toolpath you won't end up with the intended shape! What you'll need to do is create a curve parallel to and above the shape you want - the radius of your round-nosed cutter away from that surface.

Once that curve has been created, delete the original shape and do the file conversion. When you run the converted file, subtract the radius of the cutter from the z-height.

This is /almost/ intuitive (: but not always obvious. The easiest way to see why is to imagine cutting a "\" shape - and note that at no time is the bottom center of the cutter used to cut that surface!

Am I making any sense with this explanation?

...Morris

[mrdovey]

One other thing. Since you seemed to be interested in other languages for manipulating part file data, I wrote a quick and dirty C file to do the same conversion; and would be happy to e-mail it if you'd like to see what that looks like...

...Morris

[paco]

Well, I must admit that I did'nt been very clear about this in my previous post... in fact incomplete!

YES! I'm interested to obtain your converter. Thanks in advance!

[mrdovey]

Paco...

You have mail. Note that the conversion program doesn't want an END after the move commands.

...Morris

[btk]

Morris,

Can you please clarify why you generate these files programatticaly,
for example,
(a) Do you not have access to Artcam Pro (or
Rhino/MillWizzard)
and/or
(b) Do You feel that Artcam Pro or Rhino does
not do as efficient of a job in generating
the paths.
It appears that GaryB is using Artcam to
generate his toolpaths and while I agree
that when you simply want to "extrude" a profile along a simple linear path, then longitudaly would
be relative straight forward, however when the
path becomes more complex with different inversion points (as Mike Johns orignial post), then would you feel that it would still be effiecient to spend the time developing the mathematical routines.

The reason that I ask is that I have milled parts in the past like the one Mike inquired about from computed toolpaths, however I always ran latteraly, not longitudally,
However when doing something like your cove, that
has a consistent profile (or at least one that only changed linearlly) I would run the job longitudally.

[mrdovey]

BTK...

Good question. The reasons have to do with what my personal skills and talents are; and what I want to get out of my work.

[1] Every CAD package I've ever used has, at some point, thwarted at least one of my design attempts; and I finally tired of paying for frustration.

[2] I can invest my time and energy in becoming expert at using a CAD package (not becoming expert doesn't seem like a sensible choice) - or I can invest that same time and energy becoming expert at applying geometry, trig, and algebra to problem solving.

[3] I already have passable programming skills and this considerably facilitates any programatic approach.

[4] Math and programming skills, one acquired, seem to be endlessly reusable and ever easier to apply to new classes of problems. Gary's column, for example, consists of circular elements only: two cylindrical sections and a set of helices all on a common axis. The "ropes" are the result of sweeping the helical paths with a circle.

Is it more efficient to spend the time developing mathematical routines? Hmm. I guess that would depend on a whole collection of variables that you haven't stipulated - so I'll give you an answer of "at least sometimes." I'm not sure that there is any single answer that's /always/ true.

What I have found to be consistantly true is that my part programs get the job done in less time and with generally higher quality results than the canned packages produce; and when problems have arisen, I've been able to correct them /very/ much faster.

...Morris

[fleinbach]

Morris

I couldn't have said it better myself. I too still use simple and sometimes seemingly crude manuel methods to acomplish my goal. You are right, if you are not proficiant with any particular software out there manuel methods may work much faster, but then again some jobs still reguire using software to negate and grately simplify the job at hand.

[btk]

Morris,

I appreciate your answers.
I was only asking because while
I have spent considerable time in the
past generating CNC files (w/ Fortran, C, PERL etc), and I too agree that these methods give you
better ability to re-use components, modify existing designs and concepts, I just recently purchased a Shopbot (3 weeks ago) and have only recently seen demos of Artcam and Enroute, I guess I was a bit confused by the initial post in this thread as I am not yet
versed on the built-in capabilities of these
different packages (i.e. Part Wizard, Mill Wizard,
Visual Mill, Insignia, Pro, etc) and what 3-D
capability each one offers out of the box.

While I plan on purchasing either Artcam or
Enroute in the future (as I have seen things in these demos that are very intriguing), until then, (and I presume even afterwards) I will probably continue to do many tasks on the shopbot by generating files programatically.


Thanks for helping me clarify this.
Brian

[paco]

Beware of vendors... make your own mind... there's "always" demo version... or it should! It really $hould...

[jim_ludi]

Paco - Where'd you find the system variable for the cutter diamater? My programming handbook states that the system variable for the "current" cutter diamater is %(20). But, the list doesn't show variables %(23) & %(24), so... Jim

[paco]

What I'm refering to is about the PRT Alpha system variables (SB3; window version)... my programming handbook too says %(20) (old info.)... but the "ShopBot V3 System variables 09_15_04.pdf" in "\Program Files\ShopBot\Developer Tools\Docs\"
says %(23)... keep %(20) variable value if you use sb239sx_m.exe (or older?) with a PRT...

[ron brown]

Tool path in Rhino - 5/8" flat bottom bit and properly compensated, 25% bit offset.




~4 minutes cutting time at 1.50ips

Ron

[ron brown]

2673

[gerald_d]

And how much manual sand-papering time?


For those wanting to use the SB to mill it out, it must be understood that your cutter will be plunging at least 40mm deep at times. There is a lot of wood to be hacked away.

I think that the milling approaches discussed above, using a machine with 3 linear axes, to produce a cylindrical shape, is not as effective as a lathe.

If Mike wants half pillars that will match in pairs to make whole pillars, my first consideration would be to turn whole pillars and then split them with a thin blade (bandsaw). The loss of the saw-kerf should not be noticeable on a 3" diameter pillar. I think this option should be discussed first, before assuming that it is a SB job.

[ron brown]

Gerald,
I agree with your turn and split. I would split then turn. My "build it all on the ShopBot" approach would be using the approach I showed then sanding. There will be less sanding than if using a ballend bit with the same step-over. I use the "Her-Saf" brand indexable bit and the inserts cost US$0.87 or so an "edge". They seem to last a long time, longer than any other bit I have ever used.

As a production turning, once the blanks were prepared (octagional blanks [I would do this on the ShopBot too, the hell with 40mm plunge cuts] and centers marked or better still, centering holders on the lathe), those should be able to be turned at the rate of 10 or more an hour. I would not want to turn all 600 for a year in one setting as I am not pleasant to be around after a few hours of solid chip injestion.

Ron

[garyb]

Actually Gerald, sandpaper time is not much different than the lathe providing you used the correct bit and stepover rate combinaton, then tool path strategy makes a big difference in the amount of work the Z axis does.

I agree with you, that you don't assume this to be a SB job but Mikes original post stated these were currently being done on a lathe and questioned how easy they could be done on his soon to arrive SB.

I believe quite easy, as shown by the different methods and posts above.

[mrdovey]

I must be the only guy around without a lathe. (-:

If I needed to produce these things in quantity, I think I'd clamp five 8cm x 4cm x 2+m pieces at a time and cut 20 at a time. The 4cm thickness translates to a 1.575 finished thickness, so I think I'd cut the bulk of the profile for all parts with a 1" round nose bit, then remove the final 0.075" at the edges with a straight bit.

The blade currently on my table saw makes a 0.118" kerf, so three kerf widths would need to be added to each 2m blank.

I think my PRT-96 could beat your lathe production rate, provide a surface for which you'd consider 220 sandpaper coarse, and eliminate the need to stand over the job and injest beech bits.

I can see that I'm missing a lot of fun by not having a lathe in my shop. ;-)

Morris

[mrdovey]

Oops! I just realized that I can cut the whole thing with a round nose bit -- don't need the straight bit for the final pass. (-8

...Morris

[paco]

Frank (& Morris),
workin' on the "arched moulding" is quite a real fun!!!

2674
I'll be testing the program this afternoon... looking to improve a little more; mutli pass, better procedure to get to finish part and so on...

[mrdovey]

Paco...

Looks like you're having TOO MUCH FUN!

8-D

Morris

[fleinbach]

Paco

It appears your doing a spectacular job. I'm interested in seeing the final results. Maybe it could be one of the extra tools in the shopbot software. It would be great if you could insert a profile then just select whether to follow the edge or the center of your intended path.

[fleinbach]

Morris

How many passes and how long would it take to be close enough to use 220 grit paper? This dosen't seem possible considering there would have to be some material left between passes requiring a bit more then 220 grit, unless your going to be sanding for quite some time.

[gerald_d]

Maybe I have been spoilt by having access to CNC lathes long before the SB came along. We have some companies here in Cape Town who specialise in lathe work and we refer this type of work to them - they in turn refer 2D (or 2.5D) flat/sheet stuff to us. None of us breathe in chips while the lathes are doing their work (The cutting time for Mike's pillar will be around a minute or two).

Our approach to the use of the SB is probably different to most of the guys in this thread. We have identified which type of work is the most profitable (efficient) and we focus on that. The less efficient stuff we pass along to guys who pass other good stuff to us.

[mrdovey]

Frank...

[chuckling] I'm so glad you wondered! I wondered the same thing and am putting together a set of web pages with the answer. My first effort was aimed at cove (concave) profile cutting - and the current effort is round (convex) profile cutting. You're invited to take a look at the cove geometry pages with links at http://www.iedu.com/DeSoto/CNC/

The round convex problem is addressed in essentially the same way. I'll add those pages when I've had time to add some good drawings.

In a nutshell: It's possible to specify the height of the ridges you're willing to tolerate - and from that calculate the spacing between passes required to produce that height ridge. For quality parts I've found that specifying a ridge height of 0.001" generally produces a lovely finish surface on fine-grained hardwoods like cherry - with no visible ridges to sand.

The 1-1/2" radius quarter round cut into fir construction lumber posted earlier required 45 passes with a 1" core box bit. I later hand sanded the part with 220 grit paper for the time it took to warm a cup of coffee in the microwave (~90 seconds) to produce a finish surface.

...Morris

[mrdovey]

Gerald...

Lucky you! The nearest place to my shop where I can get wooden parts turned in quantity is about 70 miles away - and they're expensive!

Wishing I could be spoilt, too...

Morris

[fleinbach]

Morris

I deffinatly agree a concave surface using a wide core box bit would not leave very many ridges. This would certainly require minumal sanding. But on the other hand a convex surface would be a bit more difficult.

[mikejohn]

Hi! Gents
Let me explain why I want 2 halves.
First, its easier to get good beech 40mm thick than 80mm thick. I know I could join 2 40mm x 80mm pieces, and have them turned on the lathe.
The type of rocking horse I make last for generations. One of the weak points is the pillars to rails on the stands. After 20 or 30 years, they can weaken. I have devised a threaded rod that goes through the pillar, with a nut in a slot in the middle of the pillar. and then through holes in the rails (with an iron bar between the pillars in a groove underneath the rails) fixed with nuts. Wooden capping pieces disguise the threaded bar.
As things shrink, the cap can be removed, the nuts tightened, and the cap put back.
Rocking Horses hate modern central heating (and being fed late).
.........Mike

[gerald_d]

Why not install the nuts when you glue the planks together, and then turn to outer shape? Or, do rattling nuts bother you?


The SB will be perfect for cutting the nut pockets, the groove halves for the threaded rod, plus shallow dowel holes for locating the halves while glueing.

[paco]

Morris,
it took me about an hour and a half to fall asleep last night after I've gone to bed(1h30 AM); could'nt think of some thing else than to solve programming "problems"...

Frank,
the first tests are encouraging; just got to fix some mesuring definitions...
This part was cut in about 8 minutes; it is about 9 3/4" wide by 4 7/8" (exterior) and 1" thick with exactly the shape/profile I was looking for (from a CAD drawn curve)... done in white bead foam, with a 1/4" ball end tool... it is as smooth as my behind!!... sorry, I don't have a digital camera at hand... to show the part!!!

8oD

Here the preview from SB3...

2675

...as for now it is simple SB code programming (maybe later as "Real" program from C code with more control/possibilities); the program prompt for which file to read from (CAD drawn curve...), lenght and wideness of arc and bit size. I'm looking for to improve some more the process and adding new parameters to control the output part... maybe choosing from an arc or a circle/disk... will keep you informed...

[stickman]

Paco,

Have you wrote a program that allows you to put in a 2d profile and the allows you to extrude that along a path within shopbot? Is that what you have done in the pictures above, given shopbot a 2d profile and a path and told it to machine.

Jay

[mrdovey]

Frank...

A convex surface really isn't any more difficult than a concave one. I went ahead and uploaded the page (without the complete set of drawings} describing how to calculate convex/round cut spacing here (http://www.iedu.com/DeSoto/CNC/convex_spacing.html). Note that the two problems are remarkably similar.

[The completed web page will have a link in the CNC resource menu (http://www.iedu.com/DeSoto/CNC/), but may have a different name.]

...Morris

[paco]

Jay,
my work is, for now, along an arc (to which there is some parameters that allow some possibilities...); I'm looking to do it with a circle too to enhance to even more possibilities... From a very "distant" view, I believe it will be feasible to extrude a profile along "any" path but it's not done yet... by me! The profile to extrude can be of "any shape" done in 2D CAD... the two example I've shown so far are basic shapes for testing... I think that with more steps, one could use different tooling to create a wide variety of extrude shape...
Many things to think of; I spend most of the late days on the phone or on the Web in search for prospects customers... I get to work on thoses projects mostly at the evenning (and night)... I'm currently have another project on the way that is a "Automatic tool bit zeroing routine on a fixed Z-plate" too which is now on the testing... more later...

[fleinbach]

Paco

From what I saw I thought you where extruding to only an arc or a circle. This is half the battle. The next step would be to follow any curve. I still find it hard to believe none of the existing software availiable out there is capable of doing this. Maybe they do and I just am not aware of it. But in any case you seem to be getting the first step toward this capability. Keep up the good work.


Morris

I didn't mean to imply a convex shape would be more difficult to follow then a concave one. What I was trying to convey is that when using a core box bit to follow a concave shape the radius of the bit almost follows the shape intended. This would leave very few ridges. While following a convex shape using a ball nose, V bit, or straight bit the bit profile does not come close to the shape it is cutting therefore leaving more ridges to manually clean up.

[paul_a]

Frank

In ArtcamPro you can extrude any section through any curve or outline and then create your toolpath.

Paul

[fleinbach]

Paul

I have seen Artcam and realize you can extrude a profile and cut it. I may be wrong but it is my understanding it will only do hoizontal or diagonal tool paths across the profile raising and lowering the Z axis for the highs and lows. What I am wanting to do is follow a path with the profile with the Z axis remaining at a constant hight for each pass. This would place all lap marks from the bit in line with the profile extrusion or path. This would make it easier to remove them or in some cases they could actualy stay. Ridges following the extrusion are far less objectional then those created at various angles to the profile.

[mrdovey]

Frank...

The concave curve isn't quite as "friendly" as it would seem - and the convex shape isn't quite as "unfriendly".

Either way, it's possible to control the height of the ridges by calculating an appropriate spacing between adjacent cuts. For test parts I usually leave 0.01" ridges - and for production cutting I normally leave 0.001" ridges, which are so slight that they're insignificant in comparison to the height to which the grain is raised with the first coat of finish.

Extruding a profile is fairly easy. One needs only two "pieces" of information: [1] the shape of the profile (Paco's earlier set of M2 commands) and [2] the path over which the shape is to be extruded (another set of M2 commands will work nicely).

To cut the extrusion, sequential (x,y) pairs are taken from [1] - the x-value is used as a displacement of a "contour" line from from the path defined by [2]; and the y-value is used as the z-height for that contour.

There are two things to keep in mind: First, there may need to be some additional points added between the existing points in the [1]-profile; and second, all of the displacements need to be applied along a line normal to (at right angles to) the [2]-path. While both of these are easy to do, they're also easy to forget (:

You don't need to have ridges if you don't want 'em. I wrote a little program to calculate the cut spacing for convex (round) shapes - and when I gave it parameters for a 1.5"-radius profile cut with a 1" core box bit leaving 0.001" ridges, it gave me the following:

C:\WINDOWS\Desktop>convex 1.5 0.5 0.001
The angular displacement is 0.036503 (2.091478 degrees)

When I actually cut that shape I used 2-degree spacing and I couldn't detect any ridges at all.

...Morris

[garyb]

Frank, you are incorrect in relation to tool pathing in ArtCam. If machining a relief you can select an offset strategy and cut in climb or conventional direction and you can select a starting point of the inside (center point) or outside edge, which is what your wanting to do.

As far as lap marks from the bit, you don't get them if you use the correct bit and stepover rate. Closing the stepover rate will give you a cleaner and smoother cut but will increase the machining time.

[paco]

Frank,
it is true that machining along the extrusion curve of a such 3D part as I've done so far get you to a VERY smooth finish; I have the foam part right beside the keyboard as I'm writing this and almost ONLY light shadow can reveal the ridges... to the touch, it is very smooth; as smooth as... I have followed the machining process and the "stepover" (here, a distance that is a combination of X & Y and Z plan moves) was about 0.03"-0.05" when observed horizontaly or verticaly!!... what is even more amazing is that this same part have been machined in less than 10 minutes (8:16-8:24) at 5"IPS... I would think that if this part has been conceived in say Rhino than machined in whatever CAM (please correct me if I'm wrong) it would have take up to an hour to machine it... not that I would'nt wish to own ArtCAM PRO!!!

[paul_a]

Frank

The finish with Artcam can be very clean if machined as Garyb described, the only downside is the lack of sharp internal corners..To overcome this I plot the vectors to the internal corners then machine these with a end mill cutter parallel to the path at a constant z depth, this really cleans up the moulding.....I do agree that it would be great to machine profiles at a constant Z depth even for just time saving.


Paul

[paco]

Do ArtCAM PRO enable toolpathing with the "waterline" (constant Z height)? I thought I've saw this!?... and if so, does it gain more speed to the machining of a 3D file?

Buy the way, here extrusion on a circle shape!


2676

[fleinbach]

Garyb and Paul

I am not sure if we are all on the same page. Paul you agree with Garyb until you mention

"I do agree that it would be great to machine profiles at a constant Z depth even for just time saving."

Are you indicating Artcam does this or that it doesn't?.

Garyb says
"machining a relief you can select an offset strategy and cut in climb or conventional direction and you can select a starting point of the inside (center point) or outside edge"

My understanding of what you are saying is that you can clear an area at the same depth inside or outside of some vector at a constant Z height. I realize this but what I am describing is simular to Pacos profile just above. My question is: Can Artcam follow that profile completly around at one Z height then step over at a new Z height and go around it again?

I may be mistaken but it is my understanding that it cannot follow the profile. Please correct me if I'm wrong

[geneM (Unregistered Guest)]

Paco,
As to the origional question...
We do turnings and pilasters all the time.
the key to this, as I see it, is to "spot" glue the 2 halves together.
I can then separate them with a chisel, sharply placed on one end or the other.
when making the half pilaster on a flat 3 axis machine, the side of the bit will remove material from the design without allowing for the shape of the bit.

ARTCAM will create "offset" toolpaths as well as the standard ones.
We have used these with much success.

a question though...
in your efforts to gain speed in cutting, do you need to sand more?
I have long felt that the CNC can work for longer periods, allowing me to sand my projects less.

thanks
gene

[mikejohn]

This Z waterline was achieved in AutoCad 2000.
(Pictures a bit naff, I resized it after saving as a .gif
)
Not the original pillar, but a similar idea.

You simply need to decide how much deeper each Z cut needs to go, then identify each contour with a different colour.
2677

[paco]

Gene,
I'm not the original poster of this VERY interesting thread; it's Mike thread!
I agree that "your idea" (http://www.talkshopbot.com/forum/cgi-bin/discus/show.cgi?tpc=2&post=20050#POST20050) seem to me as the most straightforward... but Morris's method seem VERY interesting to simply do it on a 3 axis basis... hence, enjoying more the tool with it's basic equipment... (Something you want to add to this Morris?)

YES; "my effort" result's are getting me a part that is smooth as... should I take a picture of it and post?!!... thrust me; it is smooth! (http://www.talkshopbot.com/forum/cgi-bin/discus/show.cgi?tpc=2&post=20232#POST20232)... but just like you I would know what to do with spare time while a long machining process...

Assuming that PRO can machine a 3D relief as I machine the extrude shape with my program ("waterline 3D relief machining strategie"); creating each pass as a set Z contour... should'nt it machine it as fast as I do (considering the same finished part (http://www.talkshopbot.com/forum/cgi-bin/discus/show.cgi?tpc=2&post=20232#POST20232))?!?!

[fleinbach]

I believe this post contains 2 different elements. Mike started asking about turning half columns. Next Morris and Paco diverged into following a contour. Bad Morris! Bad Paco!

I must admit I was drawn into there concept since I had been contemplating the same strategy. So here we are see sawing between 3D machining and 2.5D contour following

[geneM (Unregistered Guest)]

Paco,
sorry, on a long thread as this I often get names mixed up.
I had no luck with adding paper to the blank.I do however use three or four spots of glue about the size of a half dollar, this breaks apart easily.

but when cutting these half pilasters, there is a point that a tall shoulder becomes a slope instead of a wall.

We use the raster strategy to cut our moldings and stepover at .005.
these come out easy to sand.

I am very interested in your strategy and will be glad to experiment in artcam for you and will post results. if you are interested.

Frank,
these issues are dear to us all. Radius moldings are a venue that all botters can make some serious cash on.
builders need them on almost every home.
millwork shops generally use a Williams & Hussey open molder. but they need to have cutters ground for each new profile.
the CNC on the other hand allows for almost any profile to be cut with a single bit.
and the W&H molder can only cut a radius of about 16" and will never cut a one peice circle or oval.

My dilema, as always is to try to keep all 5 of our bots going. and pushing the parts thru the sanding process.
our molding machine cuts without sanding.
but is not cost effective untill about 4 peices are ordered.
"one offs" come in the shop about once a week
the CNC is indespensablefor this.

Picture framed wall panels are becoming more popular, kind of like a mini chair rail molding with fancy corners. these corners are a nuisance to route.

I am thrilled to find this thread, probobly the best I have ever seen.
these issues are to the benefit of the entire industry.
bravo Gents.

one more thing. The forum is calling me an"unregistered guest" because I forgot my password.(silly me)

thanks to all
at your service
Gene Marshall
www.marshallsmillwork.com (http://www.marshallsmillwork.com)

[paco]

Gene,
I'll be curious about PRO's result about what I suggest...
Still when using the raster strategie, do you run it "longitudinally"; along the lenght of the moulding?
You just confirmed to me what I intend to verify monday morning; do some people are looking for curved moulding?... I had guess yes but had to verify... and still, will do...
I must admit that I ran into a limitation with my little program; I can't get it to machine an oval correctly... Here's screen shots of testing that says it all...

2678

2679
Note how the righter most extrude shape is "stretched"... this I'm working on it till this morning but did'nt find a fix for yet... I invit anyone who would like to join the "programming fun" to say so and we could share solutions from I've worked on so far ... this could be GREAT part for oval picture frame as Gene suggested...

[mrdovey]

Frank...

Yeah - OK - my bad. It's really difficult to have one of these discussions without diverging to explore new (to someone) possibilities. Had it not been Paco's moldings, it'd have been fluted columns. (-8

I'm not really sorry. Hopefully, Mike learned that the ShopBot is capable of doing what he asked about - if he wants it to.

I was goaded into adding another web page and to write a piece of software to make ropes - and find myself writing another to cut extrusions.

Paco is about to add a (hopefully) profitable operation to his operation, based on software that he's learning to write (and learning to produce one's own software as needed is no small accomplishment!)


Paco...

You *DO* need to post pictures! And yes, I'll add that after buying the PRT-96 (and indexer) I more or less lost interest in adding a lathe to the shop. I may change my mind later, but up until now I haven't needed anything more than quarter round.


Gene...

Thanks for the information. I think I may call on some of the local millwork folks and see what kind of referral arrangement I can work out for moldings and shapes that they can't (or find troublesome to) produce. (-8

...Morris

[mrdovey]

Paco...

How are you arriving at your "oval" shape? Are you calculating points around an ellipse? And how are you handling the stepover?

...Morris

[paco]

It's a circle that is use as for the path of the extrusion and to get to an oval (or elipse?!) is to stretch this circle proportionnaly in X or Y axis... the step over is from the file that is read by the program with some calculation... I'm using the same kind of "converted file" than from my previous exercises on the first program you've help me with...

Sorry Morris; I don't have a digital camera at hand for you to admire my behind smoothness!!!

[garyb]

OK Paco I believe this is the tool pathing your wanting to see, profile similar to yours above toolpathed in Artcam.

2680

The following two I believe are for Frank showing the difference in stepover to reduce the ridges thus reducing sanding.


2681

2682

[mrdovey]

Paco...

If you're simply stretching the previous shape (and its toolpaths) you're distorting the stepovers so as to prevent true extrusion.

You'll need to calculate the stepover distance along lines normal to the true shape/previous toolpath (and not from the center of the distorted circle.)

Am I making sense?

And, for the record, I'm absolutely NOT interested in your backside - not even if you plan to (or already have) reworked it on a ShopBot. |-8

...Morris

[paco]

Hummm... need more... currently testing other options...
by the way and a little out of this particular "circle program"; I did'nt yet figure how to follow say a "S" path to extrude a shape from... it it possible? From what I figured so far, I would need to get the X & Y values from a file for the path and another value (from another file) for the stepover then the same late value and a Z value for the shape to extrude?!?!? It's beginning to boil up there!!!...


Hope I did'nt offended you with my last joke?!

[fleinbach]

Garyb

I see Artcam can somewhat follow the profile but it still does not follow it perfectly at the same Z height per pass leaving ridges at an angle to the profole path. It would seem that if it can some what follow the path why can't it follow it precisly.

geneM

If I read you correctly, and I understand you use Artcam, you are saying Artcam can not follow a profile remaining in one Z height at a time creating a much desired molding shape with minumal sanding needed.

OOps! gotta go dinner time.

[mrdovey]

Paco...

No offense taken. I would like to be able to see what you've done, though. It's impressive without pictures - but pictures can carry a lot more information. If you don't have a digital camera, you might consider buying one - photos can be powerful sales tools...

Cutting the elliptical shape and cutting any shape are really the same problem with the same solution. Here are two ellipses (black) with tool paths in red:

2683
In both examples, the ellipses were constructed by distorting circle as you did.

In the upper example the toolpaths were constructed by constructing lines of constant distance from the next line inside.

In the lower example the toolpaths were circles concentric with the inner (black) circle and were distorted with the circle.

Notice how the upper (correct) toolpaths seem to change shape as you move from inner ellipse toward the outer ellipse. This isn't intuitive; but it is correct. There just isn't any other way for the profile to remain the same all the way around. As soon as you manage to internalize this (when it finally feels right) to you I predict you'll have no difficulty with the kind of distortions you've seen - and you'll have no difficulty seeing how to follow any path.

Now - ready to cut a figure 8-shaped moulding? (-8

...Morris