Good, cheap, material to practice with?

This forum is dedicated to those Hobbyists Interested in CNC machining in their home shops. (Digital Read Outs are also topical, as is CAD/CAM as it relates to CNC)

Moderator: Harold_V

dorin
Posts: 523
Joined: Thu Nov 28, 2002 5:24 am

Re: Good, cheap, material to practice with?

Post by dorin » Thu Jul 07, 2016 2:03 pm

I was able to find two giant plastic cutting boards at Goodwill extremely cheap.
13x19x5/8...seems to cut very nicely at my speeds I am at.

Thanks everybody for the advice!
-Mike
www.chaski.com

User avatar
SteveHGraham
Posts: 6854
Joined: Sat Jan 17, 2009 7:55 pm
Location: Florida

Re: Good, cheap, material to practice with?

Post by SteveHGraham » Sat Jul 09, 2016 4:43 pm

This week I bought a piece of 3/4" Delrin (acetal) rod for CNC practice. I tried it today. It's wonderful. It's way more forgiving than aluminum when the tool goes the wrong way, and the finish is incredible. I used a cheap Chinese carbide insert with a microscopic radius, and the Delrin is so smooth it looks like it was cast in a mold.
Every hard-fried egg began life sunny-side up.

GLCarlson
Posts: 1
Joined: Mon Jul 25, 2016 1:46 pm

Re: Good, cheap, material to practice with?

Post by GLCarlson » Mon Jul 25, 2016 4:39 pm

dorin wrote:I just got my little CNC sherline going!

I have been practicing with this things like this:
1) Insulation http://www.homedepot.com/catalog/produc ... da_400.jpg
(This works ok, but tends to wrap around the cutter. )

2)old PC boards.
(Which I understand will dull my cutters quickly...but they are plentiful in my house and seem nice to work with)

3) I have also messed a bit with MDF, but boy does that make a mess.

Any suggestions...Looking for something cheap that machines sort of nicely to practice with.

THank you!

-Mike
I'm a little surprised not to see a mention of pink foam building insulation. Cheap, not messy, easy to stack pieces with a little glue to make bigger pieces, and it machines very nicely. Won't dull cutters, can run g-code at high speed -which actually helps with proportionate rpm- and if one does have a bad move somewhere, the stuff just tears. Doesn't need coolant. And you can generally mount it just as you'd mount a piece of stock. A 2" thick 4x8 foot sheet is 30 bucks or so.

I've been able to cut it in the lathe and mill, even threadmilling 20 tpi threads that work. Problems: it abrades, is hard to measure without deforming, and can load up a cutter if the cutter gets hot. And it isn't really very good for small parts (under an inch or so).

Credit where due- this was a recommendation from a tech rep at Tormach. His reco was air cut then run foam. By the time you touch cutter to steel/aluminum/whatever, you'll be pretty sure your motion works. You still need to get speeds and feeds and coolant right.

User avatar
Mid Day Machining
Posts: 417
Joined: Thu Apr 09, 2009 10:58 am
Location: San Clemente, CA

Re: Good, cheap, material to practice with?

Post by Mid Day Machining » Mon Jul 25, 2016 6:02 pm

I would look for a scrap yard where you can buy aluminum solids for $1.00 to $1.50 per pound or go to some local shops and ask if you can buy some of theit scrap material.

Don't try to machine composite material with high speed steel cutting tools. That's like trying drill a hole in a grinding wheel with a plastic drill.
You can buy good parts, or you can buy cheap parts, but you can't buy good cheap parts.

User avatar
Errol Groff
Posts: 266
Joined: Sat Aug 26, 2006 8:35 pm
Location: Preston CT

Re: Good, cheap, material to practice with?

Post by Errol Groff » Tue Nov 01, 2016 9:54 am

You might try Corian the counter top material. Visit a cabinet shop and beg for cutoff scraps.

Errol Groff

RET
Posts: 718
Joined: Wed Jun 07, 2006 8:36 am
Location: Toronto, Canada

Re: Good, cheap, material to practice with?

Post by RET » Wed Nov 02, 2016 7:37 pm

Hi Dorin,

Like you, I started off with the little Sherline CNC mill at least 15 years ago. Its a good machine to learn on and I made quite a few good parts with it. It is also good value for the money and I really like the software, especially the Sherline "front end" that mates with the EMC program. As far as I can see, the Sherline CNC lathe program doesn't have that interface and it isn't as "user friendly."

I'm interested in 3 1/2" gauge and 7 1/4" gauge live steam locomotives so the parts I made (and make) are for that.

I don't really understand why you would want to use a "practice" material. Just go ahead and make the parts you want to make. Twice I made a part out of aluminum as a "test" piece, but those were the only "practice" parts I made. Most of the others have been made from steel or brass. Just remember, with the little Sherline mill, a "heavy" cut is 10 to 15 thousandths.

I started off by using Joe Martin's book to learn how to write G code (its very good), writing the code for the parts I wanted to make and going on from there. After about 10 years, I made a much bigger (2 X the travel in each axis) and heavier machine but I still used the same steppers so the Sherline software doesn't know the difference. The new machine is Much better and without the limitations of the little Sherline mill. Since it cost me $2,500.00 per axis for the ball screws and Thomson support shafts, it should be better!

There are a few things I've learned over the years about writing code for the mill. For most parts, I write the code manually. For the really complex parts I use a 3D CAD program from Weber systems called Synergy. Once I have the part properly drawn in the program, it will generate the G code to make the part. I have only done this for the Number plate for the front of Big Boy (two) and the number plates for Dart.

The other simpler parts I make by manual code writing are usually a toolpath of some kind that I gradually sink into the work with multiple passes to create the end result I need. Sometimes it will take more than one program to create the desired part. To create the toolpath, I draw the part in CAD using a 2D program called Anvil. Once the part is drawn, I make an offset line which is half the diameter of the cutter I will use to create the part. I use the CAD program to get all the intersection coordinates (and radii) of the lines that make up the toolpath. I make sure that I have at least 5 decimal places for the coordinates since the Sherline software requires this degree of accuracy.

Once I have figured out where "Home" will be on the part (I make that 0,0,0), I start writing the G code using the coordinates I obtained above. Since G code programs should start and end with the % sign, I put down one at the very start of the program and I put the other at the program end. After the % sign, I use brackets () to write comments at the start of the program because anything in the brackets is ignored. I put down things like the name of the program, the cutter diameter I'm going to use, the cutter speed, feed rates, climb milling or anything else that I would need to know if I came back to re use the program at a later date.

I write the "exit" part of the code after I've written the first few lines (use G0 & z to go high enough to clear everything, then give the "Home" coordinates). The "Home" code section is always a few spaces down from the part of the code I'm currently writing. At the start, I figure out where I want the cutter to come into the part and either do this at a corner, or use a tangent arc to come in smoothly (go out in the same way). From that point I continue to write the code for the toolpath and every few lines of code I stop and run it watching for error messages and seeing if "Backplot" gives me what I need. When you start using the rotary axis, Backplot can start looking pretty weird. By writing in this way, you get to test the code as you create it so debugging is pretty easy.

On the other hand, the Big Boy shields were not easy to debug because there were 1,600 lines you had to go through and edit. I did that by putting the % sign in every 20 to 50 lines and running the code up to that point. Once that checks out you move the % sign further along and repeat. You learn by doing. I had to change all the feeds in the program because they were commercial CNC speeds and the Sherline runs MUCH slower.

Sorry, this is a bit long winded, but I hope it helps.

Richard Trounce.
Last edited by RET on Mon Nov 07, 2016 8:04 pm, edited 1 time in total.

dorin
Posts: 523
Joined: Thu Nov 28, 2002 5:24 am

Re: Good, cheap, material to practice with?

Post by dorin » Sun Nov 06, 2016 7:23 pm

Richard,
Thank you for the long answer.

Am I understanding correctly...you generate your own g-code???
Wow I am impressed! I have thought of writing software to do that...and even started once some time ago.

What kind of spindle speeds did / do you get with your sherline?
Using the handheld tach, I don't think I cross 3,000 rpms..
-Mike
www.chaski.com

RET
Posts: 718
Joined: Wed Jun 07, 2006 8:36 am
Location: Toronto, Canada

Re: Good, cheap, material to practice with?

Post by RET » Mon Nov 07, 2016 7:54 pm

Hi Dorin,

This is going to be another "long" answer, but I hope it helps. I only really know the Sherline software, so everything I say is based on that. Since I believe you use the same software, you should be able to use what I say easily. For many items I find "Backplot" to be quite helpful. I use it to "prove" the code before actually running the machine. Running the machine clear of the part is the final test. I kept the Sherline spindle when I made the new machine and yes the spindle speed is about 2,000 rpm max, but it does the job OK. Normally, 3/16" dia. cutter shanks in the Sherline collets are the way to go because that minimizes the tool overhang. Rigidity is important. I use climb milling all the time.

Yes, for the simple parts I write my own G code. If you follow what I wrote before, its actually not too hard, especially once you do it a couple of times. Just start off with a simple part, but if possible, choose something that you actually want to make. One of the first parts I made was an expansion link cut from 3/8" oil hardening tool steel with the original Sherline mill. It was slow, but it worked just fine. One program cut the inside curved slot and a second one cut the outside profile of the link. File the ends of the curved slot square and you're done! I used the digital readout on the Bridgeport to locate the pivot holes accurately and the lower one was "Home."

Here is some of the code I wrote for 3 1/2" gauge coupler parts. The complete code occupies a full sheet of paper, so I won't give it all. This is just one of the programs necessary to finish making the coupler. The picture shows the top & bottom coupler halves mounted on the fixture I made for the part so I could go around the outside of the casting. What follows is some of the code I wrote to do this.

%
(Coupler outline top & bottom)
(use 1/8" dia. 2 flute end mill 0.5" long with 3/16" shank, Depth of cut .050")
(use feed override at 50% where cuts are heavy. Cutter gets dull after about 3 pieces and will eventually break)
(spindle speed # 7.0 - not below 5.8 with belt on small pulley step. Higher rpm. is better with 2 flutes)
("Home" is at right knuckle pin - 0,0,0)

g40 g0 g90
x0 y0 z0 a0

g0 x-2.2525 y-.025
g1 z-.950 f15.0
g1 z-1.0 f1.0
g1 x-2.2525 y.54702 f4.0
g1 x-1.54268 y.55248
g1 x-.769108 y.612916
g2 x.085366 y.852279 r.873646
g2 x.10857 y.677531 r.09536 f1.5



g0 z0
g0 x0 y0
%

As you can see, while the program is not complete, with this much, you can run it to test the code and then keep adding to the section before the space. The final bit raises the cutter clear of the part and then brings it back to Home. I use Anvil to get the co-ordinates that you see in the code. The path is a 1/16" offset (half cutter dia.) from the outside of the part.
IMGA0622.JPG
This shows the fixture that holds both halves of the coupler.
IMGA0624.JPG
This view shows the coupler parts mounted in the fixture. 0,0,0 is above the right capscrew on the front coupler half.
If you check back, you can see the code shown above follows the instructions I wrote in the previous post. If you copy it, it should run with no errors on your system because I've used the full program to complete 14 parts to that stage. I don't mind giving you the whole thing, but I want to keep this post as short as possible. Since I didn't get a reply right away, I was beginning to wonder if I had offended someone somehow so thanks for your interest. Let me know how you make out.

Richard Trounce.

dorin
Posts: 523
Joined: Thu Nov 28, 2002 5:24 am

Re: Good, cheap, material to practice with?

Post by dorin » Tue Nov 08, 2016 6:51 am

Hello Richard,
No, I had been travelling for a contract I have and it is sort of beating me down..and it was(is sort of) consuming all my time.
I am going to give this a try on Thursday when I get some shop time again.
I would not mind getting the whole program...if you don't mind. You could post it as a zip file I believe or pm me.
I am certainly going to try this as far as the program posted so far...I'll take some pictures.
I really like seeing your pictures sherline do something real!
Thank you again.
-Mike
www.chaski.com

RET
Posts: 718
Joined: Wed Jun 07, 2006 8:36 am
Location: Toronto, Canada

Re: Good, cheap, material to practice with?

Post by RET » Tue Nov 08, 2016 9:44 am

Hi Dorin,

In case others are interested, here is the whole program. For Sherline, g0 seems to be about 24 in/min. You don't have to repeat g0,g1,g2 etc. at the start of each line until there is a change, or have spaces in the code but I do that because it makes it more readable. As you can see, Sherline also doesn't need line numbers, but you can put them in if you want to. On the CAD drawing of the parts, the origin is also at the coupler pin and the drawing has the same orientation so the co-ordinates that I get don't have to be converted. Note: if an arc is more than 180 degrees, r has to be negative.

%
(Coupler Outline top & bottom)
Assume all the other stuff is here so I don't have to copy it again

g40 g0 g90
x0 y0 z0 a0

g0 x-2.2525 y-.025
g1 z-.950 f 15.0
g1 z-1.0 f 1.0
g1 x-2.2525 y .54702 f4.0
g1 x-1.54268 y.55248
g1 x-.769108 y.612916
g2 x.085366 y.852279 r.873646
g2 x.10857 y.677531 r.09536 f1.5
g1 x-.141875 y.532936
g3 x-.1575 y.50587 r.03125
g1 x-.1575 y.2512498
g3 x-12625 y.2200 r.03125
g1 x.0000 y.2200
g2 x.075246 y-.206732 r.22 f4.0
g1 x-.28727 y-.338679
g2 x-.687807 y-.151906 r.3125
g1 x-.695608 y-.130471
g3 x-.830263 y-.028139 r.15625
g1 x-1.54268 y.027519
g1 x-2.2525 y.032979
g0 z-.70 (here we move to the other part)
g0 x-2.2525 y1.5
g1 z-.950 f15.0
g1 z-1.0 f1.0
g1 x-2.2525 y2.04702 f4.0
g1 x-1.54268 y2.05248
g1 x-.83026 y2.108139
g3 x-.695608 y2.21047 r.15625
g1 x-.68781 y2.231904
g2 x-.28727 y2.41868 r.3125
g1 x.075246 y2.286732
g2 x.00000 y1.8600 r.22 f1.5
g1 x-.1262502 y1.8600
g3 x-.1575 y1.82875 r.03125
g1 x-.1575 y1.574126
g3 x-.1575 y1.54706 r.03125
g1 x.10857 y1.40247 f4.0
g2 x.08536 y1.22772 r.09536
g2 x-.769108 y1.46708 r.873646
g1 x-1.54268 y1.527519
g1x-2.2525 y1.53298
g0z0
g0 x0 y0
%

Checked, no errors! This program goes around the outside of the casting to remove the draft and to clean up the outside. There is a different program using subroutines for the coupler knuckle and there will be at least 2 more for the inside cuts. By using CNC, all the parts will be the same.

Richard Trounce.
Last edited by RET on Tue Nov 08, 2016 5:04 pm, edited 1 time in total.

User avatar
ctwo
Posts: 2618
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: Good, cheap, material to practice with?

Post by ctwo » Tue Nov 08, 2016 1:32 pm

Line 22 is going to give someone a very bad day.

g1 x-.28727 y-338679
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

User avatar
GlennW
Posts: 6609
Joined: Sun Apr 15, 2007 9:23 am
Location: Florida

Re: Good, cheap, material to practice with?

Post by GlennW » Tue Nov 08, 2016 1:43 pm

Why are you working to six decimal places?

There are many lines that way.
Glenn

Operating machines is perfectly safe......until you forget how dangerous it really is!

Post Reply