# CNC project for beginner operators ( Horizontal twin cylinder)



## stevehuckss396 (Nov 24, 2011)

Hey guy's!


I have been working 6 days a week and have had very little time for projects. I cannot find more than an hour
here or there so I decided rather than do nothing, I'm going to make a few simple things here and there.

Jimmy, One of the guy's in my club wanted me to redesign Mr. Graham's HOSC engine into a twin cylinder. I liked
it so much that I blew it up to double size and decided to build it out of Corian countertop material. Jimmy
stops in at a cabinet shop and one of the workers there gives him the sink cutouts and scraps for free. Others
have made custom pens and YoYo's and other things out of the corian to give back as a thank you for letting
us have the scraps. I'm going to build this air engine to give back to the corian guy to thank him for the
pieces I have gotten over the years. If you have seen the base plates for the Peewee and Demon and the spark
plug insulators, they were all made from this persons generosity. 

My plan is to make a part a week. With Mr. Graham's permission I will make the plans and the Gcode available
to anyone who wants to build one. The plans and Gcode will be attached to the post. I will try to get the post
up every Sunday. The plans will only contain the information required to finish the part so this will be a CNC
only thing. The CNC parts will be the base, standards, flywheel, and cylinders. The manually made pieces will
be the pistons, crankshaft parts, and finishing the CNC'd parts. 

CAUTION: The Gcode was written to be used on corian. This material is like plastic so the speeds, feeds, and depth
of cut may be way to aggressive for aluminum.







This will not be as easy as it seems. Corian has no standard thickness. I have measured pieces from .445 to .485
depending on the type and color. As the pieces are made and the project moves forward, there will be some
adjustments that have to be made. If you are the kind of person who can run into the unexpected and just roll
with it, this is your project.

First I found the center (X0,Y0) of a 7 X 5 inch piece. The top surface will be Z0 for all tools. You need to
setup this way because I wrote the code to cut .525 deep to make sure the thickness of any piece will work. You
can also stack 2 pieces on the table to protect your table when the cutter goes thru.







The holes are center drilled, and drilled with a #37 drill bit and a 1/4 inch drill bit.







Then a 1/8 inch endmill was used to cut out enough of the part to allow the next step. I know you are thinking
that a larger endmill could have been used but my mill has a small spindle motor and gets real hot with the
larger bits. I used the smaller bit and cut at 60 inches a minute and it goes fast.

Don't worry about the funny looking cut down the middle. That was operator error and not the Gcode.







A 1/16 inch radius cutting endmill with a 1/4 inch tip was used to clean up the edge. If you don't have
this cutter and don't want to buy one, you could just leave the 1/8 inch endmill in and press cycle
start. The mill will go thru all the moves and when prompted for the 1/8 endmill again, it is already in
so cycle start again and you can continue having skipped the radius step.












Then the 1/8 inch mill was loaded and the piece was cut out.







The corian is brittle so cutting the tabs with a plier caused the piece to chip. Cutting it out with a band
saw might take a bit longer but will avoid damage. I haven't figured out exactly how I'm going to feed the
air to it so that won't be addressed at this time. 

View attachment Standard.tap


View attachment Standards.pdf


----------



## chrispare (Nov 24, 2011)

Geez if this is what you do in an hour,,
nice work this is going to be a fun one.

Thanks for your spare time work and sharing with the rest of us!


----------



## stevehuckss396 (Nov 24, 2011)

chrispare  said:
			
		

> Geez if this is what you do in an hour,,
> nice work this is going to be a fun one.
> 
> Thanks for your spare time work and sharing with the rest of us!



I draw and do the Gcode in the house while I'm watching the tube. I think it took just over an hour to make 3 of these pieces.

That's something I forgot to mension about the CNC. If you go to all the trouble to setup, make 2 or more of what you need if material allows. The first one might take 30 minutes but the next 3 might take another 30 minutes. If you make a boo boo, you already have another.


----------



## Path (Nov 25, 2011)

This is going to be fun to watch and build. 


Thanks,


Pat


----------



## steamer (Nov 25, 2011)

Bubba , this is a damn fine idea!  

You sir are a genius! :bow: :bow:

Dave


----------



## kjk (Nov 25, 2011)

This is a great idea. I'm just about to start learning cnc at a local maker's co-op. What software do you use Steve? I still have an opportunity to influence what software tools the co-op gets. I know we have some donated licenses from Solidworks and AutoCad, but no one has mentioned a CAM solution. The mill is a Tormach 1100.


----------



## stevehuckss396 (Nov 25, 2011)

steamer  said:
			
		

> Bubba , this is a damn fine idea!



Thanks Steamer!

To Path (who sounds like he might actually build one) and anybody who does make one, I encourage you to post your pix of finished parts in this thread along with mine. Post the pix to show your success but also show the failed attempts so we can learn from them along with you. There seems to be alot of new CNC mill owners here lately so lets all help each other out. 

The idea of this thread is to concentrate on one piece at a time. Show pix of how you did and help each other out. Then try to apply what we learn to the next piece and see if that one comes out better than the last. I'm no CNC expert so I hoping to learn some tricks here also. I'm going to use some simple fixtures to make the cylinders and flywheel. They will be made from corian also and only need to last long enough to make a dozen pieces. I'll show how I go about doing things but if you have an idea of a different or better way, pipe up and show it.

I could post some pix of the finished parts and blast thru the build but I see an opportunity here to share and gain something here so. . . . 

Anybody going to try this thing?


----------



## Mosey (Nov 25, 2011)

Which handle is the CNC one? I only have 3 handles on my machine. ( I'm jealous).


----------



## stevehuckss396 (Nov 25, 2011)

Mosey  said:
			
		

> Which handle is the CNC one? I only have 3 handles on my machine. ( I'm jealous).



You would have to ask GBritnell on that one. He seems to have found it.


----------



## stevehuckss396 (Nov 25, 2011)

Finished the first pieces today. After getting the waste cut off I had 2 pairs that didn't seem to match. It is
extremely important that the two crankshaft holes be the same height off the base. If you have any reason
to believe that the two pieces don't match, put a couple of 1/4 inch drill bits into the 2 holes and take a 
skim cut to get them perfect.







I made a few extra pieces so i needed a way to setup the pieces quickly for drilling. Using a scrap piece of
Corian I milled the entire piece flat and then cut a slot 1/8 inch deep to use as a setup block. 







Now I can but the piece into my stop and then push the piece up to the setup block that is sitting on the
vise jaws. Should get every piece into the same place and nice and flat to within a few .001's every time.







I drilled all the left sides and then switched to the rights. The piece is left overhanging the vise so I could
get my finger under the piece to press it into the under side of the setup block.











I chucked an 8-32 tap into my battery drill and ran threads into all the pieces. Then the holding tabs were
ground off and polished with sand paper. I try to leave my tabs at high spots or corners because it makes it
easier to clean them up after.







Next piece will be the base a week from tomorrow. Until then i have alot of tabs to grind and polish.


----------



## Tin Falcon (Nov 25, 2011)

Looks great Steve I am trying to talk myself into this build should be relatively easy yo do as you are doing the R&D and blazing the trail thanks for sharing. 
I do want to reminds folks of safety. the MSDS sheets for Corian are a bit long (7 pages)and confusing here if anyone wants to read it. 
http://www2.dupont.com/Surfaces_Commercial/en_US/assets/downloads/pdfs/COR001_CORIAN_MSDS.pdf
the basics 
1) collect dust at the machine. 
2) clean up dust in the shop.
3) do not breath dust. 
I have done a fair amount of Corian work here are my methods
Keep the shop vac hand and collet chips as produced if possible. Collects dust and keeps the tool cool.if the tool gets hot the colors turn milky . 
vac up around the machine after the parts are made. 
wear a dust mask if the stuff is flying. 
wet sand Corian it keeps the dust down and he surface cool .
Tin


----------



## Tin Falcon (Nov 25, 2011)

this may be a dumb questions Steve but it seems like you have a lot of extra material around the palr. How necessarily is the 5x 7 ? I know you have it up on blocks and need some clearance on the ends so your tool holder does not hit the clamps but why so much on the y is it needed for support. I have a bunch of Corianin 4 - 4 1/2 inch strips so am thinking of using that. May clamp to the table with a sacrifice piece under it. 
tin


----------



## stevehuckss396 (Nov 25, 2011)

Tin Falcon  said:
			
		

> this may be a dub questions Steve but it seems like you have a lot of extra material around the par. How necessarily is the 5x 7 I know you have it up on blocks and need some clearance on the ends so your tool holder does not hit the clamps but why so much on the y is it needed for support. I have a bunch of corianin 4 - 4 1/2 inch strips so am thinking of using that. May clamp tot he table with a sacrifice piece under it.
> tin




You could probibly go as slim as 3-1/2. Just want to make sure it stays together while the piece is getting cut. I just happened to have a 5 inch piece here. 

4-1/2 would work well for the base also which is the next piece that will be made.


----------



## steamboatmodel (Nov 26, 2011)

Mosey  said:
			
		

> Which handle is the CNC one? I only have 3 handles on my machine. ( I'm jealous).


Its the one with $$$ on it. CNC is great, you can fill a scrap bin in no time, and come back later and refill it with identical parts.
Regards,
Gerald
Retired CNC Technician.


----------



## stevehuckss396 (Nov 27, 2011)

Tin Falcon  said:
			
		

> What software do you use Steve?The mill is a Tormach 1100.
> 
> Steve is using CAM BAM for the CAM I would expect Mach 3 for the CNC.
> Tin



I use Alibre to design and create the DXF (2D) and STL (3D) files.
Sometimes I use AutoCAD to modify the DXF's 
Then I use CamBam to create the Gcode
Mach3 runs the mill and if I ever get around to it, the lathe.

There is a free program called DeskEngrave that is good for creating and engraving text.


----------



## Tin Falcon (Nov 27, 2011)

Mosey no need to be jealous CNC is just a different way of spending hobby time and money. It can be a faster way of making parts and open new possibilities. And it can reduce tooling needs. but it is a different learning curve. I big part of me wishes I waited and bought a second mil to turn to cnc. but all learning is good. 
like anything else if the want to is there you can do it.
and like Gerald said you can scrap parts faster as well. 
Tin


----------



## stevehuckss396 (Nov 27, 2011)

Tin Falcon  said:
			
		

> and like Gerald said you can scrap parts faster as well.



Another reason I thought this would be a good CNC start. Corian is cheap and sometimes free. If you make a bonehead move (and I have) you might have a shot at not breaking the tool. I plunged an endmill straight thru a 1/2 inch thick piece because I forgot to reset Z to zero after a tool change. The mill and tool were fine and no damage to anything but a piece of Corian.

Anybody besides Tin going to build?

Friday after work I'll post the base with the code and PDF drawing. I'll do a friday post every week so you will have the info for the weekend.


----------



## Jeremy_BP (Nov 27, 2011)

I'll certainly give this a go when (if) I finish my CNC mill build.
Looks great so far!


----------



## chrispare (Nov 27, 2011)

I am waiting on a chip for my board, once im back up I will give this a go as my first cnc project.

Its quite ironic, An alumn chip somehow found its way to the stepper chip pins and shorted it out.


----------



## kvom (Nov 27, 2011)

A few comments and questions:

1) Any chance you can supply the CamBam files those of us that have the program?

2) I assume you set the tab height tall enough to account for the thinnest Corian you're likely to get. Otherwise the tabs could be quite fragile.

3) I recently acquired a quite large piece of Corian. I have been thinking of cutting some pieces up to use as fixture plates for milling metal parts.  Any reasons not to try this? I assume I can cut it easily with a jigsaw.


----------



## Tin Falcon (Nov 27, 2011)

> Any reasons not to try this?


IMHO unless it is a really boring color use it for engine bases , or even better cool engines or pen and pencil sets. 
Corian is an opaque plastic in the Methleacrelate family think lucite , perplex etc. you can pretty much use woodworking metal working tools on it. I have cut it on the table saw, band saw . turned on the lathe. heavy feeds will chip it. Hot tools will make colors milky.
Tin


----------



## stevehuckss396 (Nov 27, 2011)

kvom  said:
			
		

> 1) Any chance you can supply the CamBam files those of us that have the program?
> 
> 2) I assume you set the tab height tall enough to account for the thinnest Corian you're likely to get. Otherwise the tabs could be quite fragile.
> 
> 3) I recently acquired a quite large piece of Corian. I have been thinking of cutting some pieces up to use as fixture plates for milling metal parts. Any reasons not to try this? I assume I can cut it easily with a jigsaw.



1) I cant attach a cambam file to my post. Took a few days to get TAP file approved. You shouldn't need it with the Tap being available.

2) Tabs are plenty wide and tall. Unless your sheet get as thin as .400 you should have no trouble.

3) The only trouble you might have is threads would wear out faster than aluminum. I would hate to waste it that way. I use it as decoration and engine bases. I think it's nice looking stuff.


----------



## kvom (Nov 27, 2011)

My piece is 2x3 foot rectangle, so plenty left for engine bases. I generally use through bolts for fixtures, so threads wouldn't be a problem.


----------



## Path (Nov 28, 2011)

Steve,

I'm in the build. 

But before I can start I need to finish my part for the Radial team build. 
Cylinders and Liners are done, should have the Pistons done ... soon. Murphy is really 
getting in the way. Plus we are having some problem with the crankcase builder. He commented 
to the project but we haven't heard from him for sometime now. So we don't really know
what is going on ... hope everything is okay with him.

This project looks very interesting ... I would like to find some Corian, if not I may
use Aluminum. I did reviewed your g code by CamBam ... I will need to modify it so that it will work on my CNC.
But I don't see this as a problem ... the basic code will work (G00, G01 etc.). Just need 
to add a few things. 


Pat


----------



## Tin Falcon (Nov 28, 2011)

well I cut 4 blanks last night about 4 1/2. the downstairs bench needed a good vacuum cleaning anyway. 
need to decide what to do for tooling I am contemplating some tool holders drill holders so I do not to keep from having to reset the z on each tool for each part.
Tin


----------



## kvom (Nov 28, 2011)

On my mill I need to reset Z on endmills each time. For drills, I have a keyless chuck; to set Z0, I open the chuck and let the drill bit touch the work surface, then tighten. That's quite fast.


----------



## stevehuckss396 (Nov 28, 2011)

kvom  said:
			
		

> On my mill I need to reset Z on endmills each time. For drills, I have a keyless chuck; to set Z0, I open the chuck and let the drill bit touch the work surface, then tighten. That's quite fast.




I do the same thing. It's so fast to just touch off the tool and zero out Z.


----------



## Gerry Sweetland (Nov 28, 2011)

Hi Steve,
Thanks for providing the R&D and the build thread for this project, great idea.
I'm bummed because I just thru away 8 pcs. of 1/2" X 6" X 36" white Corian that have been laying around in my shop for almost twenty years 
I figured if haven't used this stuff yet I never will and it seemed like I was always moving it looking for something else.



			
				Woodguy  said:
			
		

> This is a great idea. I'm just about to start learning cnc at a local maker's co-op. What software do you use Steve? I still have an opportunity to influence what software tools the co-op gets. I know we have some donated licenses from Solidworks and AutoCad, but no one has mentioned a CAM solution. The mill is a Tormach 1100.



Woodguy, Just to interject here, I use SprutCam and really like it. If your Co-op bought the mill from Tormach they should be able to get a discounted price on SprutCam.
There is a steep learning curve at the beginning but once you get going it is pretty easy and versatile software.

Gerry


----------



## stevehuckss396 (Nov 28, 2011)

Gerry Sweetland  said:
			
		

> I'm bummed because I just thru away 8 pcs. of 1/2" X 6" X 36" white Corian that have been laying around in my shop for almost twenty years




That stinks. I horde white for making sparkplug insulators. Maybe you can get a chunk somewhere and join in. Would have looked great in white.


----------



## stevehuckss396 (Dec 2, 2011)

This weeks part is going to be the base.

The setup for the base is the same as the standards. I used a 7 X 4-1/2 inch piece. The center of the piece
is ( X0,Y0 ) and the top surface is Z0 for all tooling.








Once again the holes are spotted and drilled using an 11/64 drill bit.







Then enough material is removed to enable the edge to be rounded over.







The bit needed by the Gcode is a 1/8 radius with a 3/8 tip.












And then the endmill cuts out the part.







Again the waste is removed and the tabs cleaned up







Then the 4 holes that the standards are attached are counterbored.












View attachment Base.pdf


View attachment Base.tap


----------



## 1hand (Dec 2, 2011)

Steve would I be able to run your code in my Mach 3 as is?

If I where to make from aluminium can I adjust the speeds and feeds or is that all ready wrote into your gcode? I know when you made that gcode for me on the team build for the fly wheel lettering, I ran it as is without a problem.

Matt


----------



## stevehuckss396 (Dec 3, 2011)

1hand  said:
			
		

> Steve would I be able to run your code in my Mach 3 as is?
> 
> If I where to make from aluminium can I adjust the speeds and feeds or is that all ready wrote into your gcode? I know when you made that gcode for me on the team build for the fly wheel lettering, I ran it as is without a problem.
> 
> Matt



The code was written for the mach3 machines. Most people who convert or scratch build a CNC machine, including myself, so that is the target audience.

I wrote the code to cut .100 at 60 inches a minute. If i tried to do that in aluminum on my little mill it would probably tip over. I would not recommend it. If you are a CamBam user I can send the file so you can make the necessary adjustments.


----------



## gld (Dec 3, 2011)

I'm in, but lagging behind. Just found this thread a couple days ago...

Destroyed the spindle on my cnc last summer doing a freebie, and had not replaced it, so Friday i ordered a Taig spindle Assembly. Should be here next week. No Corian in his area, will have use something else.

Had to work on your code to get to work with my Deskcnc software and controller. Put the Dremel back on and cut the standards out of Styrofoam to test the code...worked great.

Thanks for posting this project....it's going to be fun.


----------



## stevehuckss396 (Dec 4, 2011)

Gary Davison  said:
			
		

> I'm in, but lagging behind.




Glad to hear your in. I just checked and CamBam won't post to DeskCNC. 

Try going to your local cabinet shop and show the guy what your going to use the Corian for. Offer to make one for him if he gives you some scrap pieces. Most guy's will after they find out what it's for.


----------



## Tin Falcon (Dec 4, 2011)

Well steve: I cut 4 blanks last weekend. I have been digging through my small collection of end mills . Do not see anything I am sure of using. I am thinking carbide with a 5/8 or 3/4 cut length Two flute end mill. I may order a few from mcmaster car but want to make sure I order what is needed. A buddy at works has offered me tooling he has a lot he is not using but has not come through yet. So forward movement is slow here. Thanks for the work you are putting into this thread . 


All : for those who are curious about cnc and want to look at the g code. you can open it up in notepad and read it through if you have other than mach 3 you or you want to edit for other material you can edit it with notepad as well. 
tin


----------



## stevehuckss396 (Dec 4, 2011)

Tin Falcon  said:
			
		

> I have been digging through my small collection of end mills . Do not see anything I am sure of using.




I use 1/8 shank carbide cutters with a .500 depth of cut. If you go with a 3/8 shank HSS then make sure the DOC is at least .750. When you get to the flywheel the spokes are cut from the top all the way thru the piece so the cutter goes .700 deep. That leaves very little clearance for the shank. If you get a 1/8 shank cutter the DOC only needs to be .500 because the deepest step is only .468.


----------



## Tin Falcon (Dec 4, 2011)

Thanks steve: I will probably order s few cutters. I do have a couple double ended cutters with 3/8 shank may be enough to get started with. 
Tin


----------



## gld (Dec 4, 2011)

stevehuckss396  said:
			
		

> Glad to hear your in. I just checked and CamBam won't post to DeskCNC.



Code change is minor. At each tool change I have to insert a M5 to turn off spindle and a G0 X0 Y0 to return to the start position.


----------



## stevehuckss396 (Dec 4, 2011)

Good news!!


I was going to engrave a few things today and then make a few engine pieces today. Half way thru the second engraving flames shot out the bottom of the spindle motor and then it stopped and made some smoke. If I knew I would only get a few thousand hours and 3 years of abuse out of it I would have never gave the guy the 8 bucks for it. ;D ;D

I just ordered a replacement motor that is about the same diameter but longer so i will need to do some reconfiguring. This should not effect the thread here unless the shipping takes forever.


----------



## gld (Dec 8, 2011)

Hi Steve

My 1/8" corner rounding end mill has a 1/4" tip.....would you please post the outline dimension's of the base(or the dxf) so I can redo that section of code.

Thanks 

Gary


----------



## Tin Falcon (Dec 8, 2011)

I was in northern Jersey today for a job found myself near McMaster Carr so 20 minute wait and $XX later I have a 1/16 rounding bit and a couple of premium grade 1/8 carbide cutters. 


Gary : I think if you want to use an 1/8 radius cutter you should be able to just edit the code run the cornering cycle twice and the second pass change the z. you should be able to do a little copy , paste and edit. But I am just learning too so if I am wrong please someone correct me. 
Tin


----------



## stevehuckss396 (Dec 8, 2011)

Gary Davison  said:
			
		

> Hi Steve
> 
> My 1/8" corner rounding end mill has a 1/4" tip.....would you please post the outline dimension's of the base(or the dxf) so I can redo that section of code.
> 
> ...



This took all of a minute and I cant post a DXF file.


View attachment BaseWith.250TipRadiusMill.tap


----------



## kvom (Dec 8, 2011)

My experience is that corner rounding bits need to be "fine tuned", and the DOC may vary. One approach is to set Z0 a bit higher than the surface and run several times decreasing Z0 until you get the desired profile.


----------



## stevehuckss396 (Dec 8, 2011)

Tin Falcon  said:
			
		

> I was in northern Jersey today for a job found myself near McMaster Carr so 20 minute wait and $XX later I have a 1/16 rounding bit and a couple of premium grade 1/8 carbide cutters.
> 
> 
> Gary : I think if you want to use an 1/8 radius cutter you should be able to just edit the code run the cornering cycle twice and the second pass change the z. you should be able to do a little copy , paste and edit. But I am just learning too so if I am wrong please someone correct me.
> Tin



What will happen is the code being written for the .375 tip, the center of the tool will run .1875 offset from the edge of the part to round over the top edge. If the .250 tip mill is used, the tool will still be run .1875 from the edge so the tool will be .0625 from the edge. The depth will still be correct. I have rewritten the code for Gary's cutter so it will be held .125 offset from the the edge of the part.


----------



## stevehuckss396 (Dec 8, 2011)

kvom  said:
			
		

> My experience is that corner rounding bits need to be "fine tuned", and the DOC may vary. One approach is to set Z0 a bit higher than the surface and run several times decreasing Z0 until you get the desired profile.



I didn't go cheap (never do on cutters) and I just cut the depth of the radius and use the tip diameter as the cutter diameter in CamBam and I get a good corner.


----------



## gld (Dec 8, 2011)

Thanks Steve


----------



## Tin Falcon (Dec 9, 2011)

> By Steve from post# 1 A 1/16 inch radius cutting endmill with a 1/4 inch tip was used to clean up the edge. If you don't have
> this cutter and don't want to buy one, you could just leave the 1/8 inch endmill in and press cycle
> start. The mill will go thru all the moves and when prompted for the 1/8 endmill again, it is already in
> so cycle start again and you can continue having skipped the radius step.






> from post #43 : What will happen is the code being written for the .375 tip, the center of the tool will run .1875 offset from the edge of the part to round over the top edge. If the .250 tip mill is used, the tool will still be run .1875 from the edge so the tool will be .0625 from the edge. The depth will still be correct. I have rewritten the code for Gary's cutter so it will be held .125 offset from the the edge of the part.


Ok the rounding mil I purchased is a 1/16 radius with a 1/4 tip so what code am I running for this ???
Tin


----------



## stevehuckss396 (Dec 9, 2011)

Tin Falcon  said:
			
		

> Ok the rounding mil I purchased is a 1/16 radius with a 1/4 tip so what code am I running for this ???
> Tin



EDIT!!! The 1/16 rounder is for the Standards ( first pieces) so the original code is what you want. The base has a 1/8 inch radius.


----------



## Tin Falcon (Dec 9, 2011)

so I need another rounding bit. There goes next weeks allowance :
Tin


----------



## stevehuckss396 (Dec 9, 2011)

This week is going to be the crankshaft. The shaft itself is made from 1/4 inch tool steel (drill rod) as is the
crank pins from some 1/8 inch. The crank disks can be made from anything you have handy. Steel, brass,
aluminum are all fine but I figured if i'm going to build a corian engine, I'm going to make the disks from
the same material. 

I had a 8 X 2-1/4 inch piece but a 7 X 1-3/4 would be big enough. The spot drill, 1/8 and 1/4 holes are drilled
as usual.








I have 5 different thicknesses of material to cut. The thickness of the finished part depends on how far from
the bottom of the stock I cut to. I have to stop .188 inches from the bottom. I cant touch the tool off the
bottom of the stock. I could write a separate program for each thickness. OR! what I did was write a program
for a .500 inch thick piece. Now all I need to do is measure the actual piece. This one was .4775 thick. That
means that the surface of the actual piece is below Z0. .4775 - .5000 = -.0225. The surface is twenty two 
and a half thou below Z0. I touched the top surface of the material with the tool and then in the Z DRO I typed
-.0225 and hit enter.







The pieces will then be cut to thickness and then cut out and drop right out the bottom. I made the program
take care of 4 pieces at a time. The thinking is that most people will make 2 or more engines.







Pretty darn close. just to recap

1) Touch tool to top surface
2) Measure stock thickness
3) Stock thickness - .5000 = Z
4) Type Z into the Z axis DRO and press enter (don't forget the minus sign for negative numbers)







I used my slotted piece for a drilling fixture. The slot was opened up to a few thou wider than the disk and a
1/8 inch pin was drilled in on center.







I was able to load and unload the disks quickly for drilling.







I then chucked a piece of drill rod into the lathe. The disk was put onto the rod and cut to finished size.







I tried to slip the drill rod thru the standards. It went thru the first one but got tight going thru the other one.
I chucked it in the lathe and polished it with some 320 grit until it was a nice fit. The shaft was then cut to
length. I measured the distance between the standards and added .389. The flats were milled into the shaft 
to complete the job. 







The crank pins were polished on one end to slip thru a 1/8 hole nicly and left to size on the other end. The big
end is then pressed into the disk. The disks are then installed onto the shaft with some 4-40 set screws.








View attachment Crankshaft.pdf


View attachment CrankDisk.tap


----------



## stevehuckss396 (Dec 9, 2011)

Tin Falcon  said:
			
		

> so I need another rounding bit there goes next weeks allowance :
> Tin



Not really. You could always skip the step and leave the top edge square. If you want I could write you a custom code to give a 1/16 edge instead if the 1/8. Only take me a few minutes.


----------



## Tin Falcon (Dec 9, 2011)

> If you want I could write you a custom code to give a 1/16 edge instead if the 1/8. Only take me a few minutes.


That would be cool. Thanks for all the work you are putting into this. Hopefully one day in the not too far future I will be able to do all the steps myself. 

As far as the crank disks go , In my experience a plastic crank dis is not the best way to go, I have made a few engines, Some of them have logged quite a few hours typically 8-16 hours a show 2 -4 shows a year some since 2003. the only engine part I had fail on me was a crank dick from plastic. I love Poly(methyl methacrylate) as an engine material both in the clear plexiglass form and the colored cousin Corian. I have made several engines with this material . FYI I have used brass pen tubes to line bush around the crank shaft the tubes are 1/4 ID and 7mm od.

Tin


----------



## stevehuckss396 (Dec 9, 2011)

Tin Falcon  said:
			
		

> That would be cool. Thanks for all the work you are putting into this. Hopefully one day in the not too far future I will be able to do all the steps myself.
> 
> As far as the crank disks go , In my experience a plastic crank dis is not the best way to go



If I were going to run them alot I would make them in brass. The engines will most likely end up on a shelf as a trophy as I am making them for the guy who supplies all the free corian. I'm guessing they will end up on his desk and run 4 times a decade.

Here is the custom base code. 1/16 radius cutter with a 1/4 inch nose 

View attachment BaseTinSpecial.tap


----------



## Tin Falcon (Dec 9, 2011)

> I'm guessing they will end up on his desk and run 4 times a decade.


Then the corian is probably fine



> Here is the custom base code. 1/16 radius cutter with a 1/4 inch nose


I thank you and my wallet thanks you. :bow:
Tin


----------



## Tin Falcon (Dec 13, 2011)

Well guys I finally got up the nerve to hit the start button. I did my homework ran the program on the laptop to familiarize myself with it. ran the program a over the work piece(set the z 0 about 3/4 above the work) cut a little air. I cant say the attempt was a failure . It was a learning experience . It did not produce a usable part. 
Some of the points learned. Remember to reset the z for each tool did it but had to remind myself
corian can be abrasive and jamb up the works put the way covers back on the mill.
this caused missteps and threw off the Zero points. 
also if you think the cutter is pushed in tighten it up it is telling you it is loose nicely. if you do not listen it will pull out embed itself in the work and break off and possibly damage the collet holding it. did i listen to the hint NO and I paid. a new end mill broken. aaarg. 
Steve: you did say post the failures so there it is. 
Tin


----------



## stevehuckss396 (Dec 14, 2011)

Tin Falcon  said:
			
		

> Steve: you did say post the failures so there it is.



I happens to everybody. I hold my endmills in collets because they seem to hold better than a drill chuck. Also run your spindle as fast as you can. I ran mine at 4000RPM. 
Also use the shop vac while you cut and all the chips are cleaned up as they are made.
Also try to Zero your tool at the same spot (roughly) on the work piece.
Also never buy just one cutter at a time. Saves alot of gas. 
What is the max feed rate of your mill when you tuned your motors and calibrated your axes. I over motored my mill a little and am able to move 350 IPM without losing steps.
This is where you become one with the mill. You learn what it likes and what it doesen't like. Very important when you start producing your own code. Once you get going your going to love this stuff!!  Hang in there.


----------



## Tin Falcon (Dec 14, 2011)

> I hold my endmills in collets because they seem to hold better than a drill chuck.


Yep did that guess I needed it tighter 


> Also run your spindle as fast as you can. I ran mine at 4000RPM.


the code said 1000 thought that seemed slow for 1/8 especially carbide now you tell me. 



> Also never buy just one cutter at a time. Saves a lot of gas.


Yeah I know I bought two wish now I got 3 . I need to place an order to Richon and order a dozen. 



> What is the max feed rate of your mill when you tuned your motors and calibrated your axes?


I do not remember I think I kept it fairly conservative the X2 has a 4x 8 work envelope so not far to go in any direction.


motors from HOMESHOPCNC are 300 OZ motors wound to match the G540/G20/g251 family.


> Hang in there.


Definitley. I have been messing with this thing for 3 years now a bit there and there. Mostly building tinkering. I am not giving up know.
There have been times I have been tempted to remove the motors and put the handles back on. but this is not one of those times. in spite of not getting a useful part the first run in full cnc mode was fun . I do need to learn to listen closer and heed what the machine is telling me . it was talking I did not listen. 

Thanks for your code and your encouragement. 
My biggest concern now is whether the collet was damaged and if it will hold a new mill. I looks a bit deformed it is an er style
Tin


----------



## stevehuckss396 (Dec 15, 2011)

Tin Falcon  said:
			
		

> Yep did that guess I needed it tighter the code said 1000 thought that seemed slow for 1/8 especially carbide now you tell me.




That is my fault!! I control my spindle with a VFD. You can set spindle speed in CamBam but I dont fool with it. Default is 1000. 

I have no idea what speed my spindle is turning. I adjust by the sound. Drilling is about 1/4 of max but the larger the bit, the slower i go. The same applies to cutters. The larger the cutter the slower the spindle speed. Like I said before, you need to find what the mill likes.


----------



## GailInNM (Dec 15, 2011)

Tin Falcon  said:
			
		

> Well guys I finally got up the nerve to hit the start button. ........
> Tin



Tin,
It gets worse when you are nearing the last operation, you have had 13 setups and have over 30 hours invested in the part. A simple "Ah shucks" will not cover the situation.
Gail in NM


----------



## stevehuckss396 (Dec 15, 2011)

GailInNM  said:
			
		

> It gets worse when you are nearing the last operation, you have had 13 setups and have over 30 hours invested in the part. A simple "Ah shucks" will not cover the situation.



Yeah but other than that, it's fun!! ;D ;D ;D


----------



## Tin Falcon (Dec 15, 2011)

> I have no idea what speed my spindle is turning. I adjust by the sound. Drilling is about 1/4 of max but the larger the bit, the slower i go. The same applies to cutters. The larger the cutter the slower the spindle speed. Like I said before, you need to find what the mill likes.


well i should have done the calculation I know 1000 is slow for an 1/8 carbide cutter. My spindle is a Pulse width modulator . I do have a laser hand held tach they are cheap. 



> Tin,
> It gets worse when you are nearing the last operation, you have had 13 setups and have over 30 hours invested in the part. A simple "Ah shucks" will not cover the situation.
> Gail in NM


This is true and can happen with manual operations as well. to err is human to realty foul things up requires a computer. I am past the point of no return. I either push forward, go backwards, or stand still and have a large expensive paper weight on my desk. so forward I go. 
Tin


----------



## dreeves (Dec 15, 2011)

Are you going to run bushings for the crank in the corian?? If not you might want to thinks about it.

Dave


----------



## Tin Falcon (Dec 15, 2011)

I typically use a piece of pen tube brass 1/4 ID 7MM OD but I need to get usabnle parts first . I may thorw a 7 mm bit in on my next try. 
Tin


----------



## kvom (Dec 15, 2011)

I consulted G-wizard for a 1/8" 2-flute endmill in acrylic with 1/2" stickout, and for slotting got 4000 rpm (my max), .24 max DOC, and 14ipm. I increased the machine limit to 10k rpm and it liked that too. So use your max rpm. Change all the S1000 codes in the file to whatever your max is, assuming PC control of the spindle.


----------



## chrispare (Dec 15, 2011)

Ok Steve I gotts a question for you.
I got a few minutes to myself today and decided to try your code for the base.
It runs good untill i get to a particular point in the code..                  


G1 Y1.469
G2 X-1.375 Y1.8314 I0.3624 J0.0 this is left corner
G1 X1.375            this is top edge  
G2 X1.7374 Y1.469 I0.0 J-0.3624 when the machine hits this line x axis stalls every time,unless i slow to a stall 
G1 Y0.531

now if i slow it down to like 1in per min it will run through then I can speed back up till it hits it again (that top right corner)
even if I move the x/y to a different position and try that code it stalls.

any ideas??


Chris


----------



## RonGinger (Dec 15, 2011)

when I try that piece of code I get the error 'radius to end of arc differs from radius to start' and mach hangs. 

I think mach should stop completely, in fact it shouldn't even let you start to run, it should see the error as it reads the code.


----------



## chrispare (Dec 15, 2011)

ok this is the piece of code that is stalling
G1 X-1.6775 Y-1.8187
G2 X-1.8125 Y-1.6187 I0.3025 J0.3497
G1 Y-1.9065
G1 X-1.5247
G2 X-1.6775 Y-1.8187 I0.1497 J0.4375
G0 Z0.025
G0 X-1.6121 Y-1.7431
G1 F10.0 Z-0.1
G2 F60.0 X-1.7374 Y-1.469 I0.2371 J0.2741
G1 Y1.469
G2 X-1.375 Y1.8314 I0.3624 J0.0
G1 X1.375
G2 X1.7374 Y1.469 I0.0 J-0.3624
G1 Y0.531
G1 Y-0.531

it stalls third line from the bottom


----------



## kvom (Dec 15, 2011)

Sounds as if the CamBam arc mode differs with the controllers. Usually for mach3 it's set to Absolute rather than Incremental.


----------



## RonGinger (Dec 16, 2011)

That longer block runs without error on my machine. 

Mach by default uses incremental IJ mode and thats what this code is doing.

Tell us more about what you mean by stalling. Does the feed rate DRO show a low value? Is the tool still moving? Does it eventually finish OK?


----------



## kvom (Dec 16, 2011)

I checked my Mach config and IJ mode is indeed incremental; it's distance mode that's absolute.


----------



## stevehuckss396 (Dec 16, 2011)

kvom  said:
			
		

> I checked my Mach config and IJ mode is indeed incremental; it's distance mode that's absolute.




That would be correct as cambam is configured the same. Take a look in the general config in the config menu and check to see if you are setup for these settings. If you change them, exit mach3 and then rerun the program again. Most times its unnessary but some things you just have to do it so now I just do it after making any changes.


----------



## stevehuckss396 (Dec 16, 2011)

RonGinger  said:
			
		

> when I try that piece of code I get the error 'radius to end of arc differs from radius to start' and mach hangs.
> 
> I think mach should stop completely, in fact it shouldn't even let you start to run, it should see the error as it reads the code.



It must be a setup thing. I used the code to make 10 pieces.


----------



## stevehuckss396 (Dec 17, 2011)

This week will be the flywheel!

I started out by cutting 3 pieces, 3 inches square. They only need to be rough sawn. There is no advantage
to trying to make 3 perfect squares. 







Sand the pieces up with some sort of paper or scotchbrite pad to remove the glossy surface. Create a surface
that will allow the glue to stick. I used the superglue gel. I completely covered the surface of one square on both
sides and sandwiched it between the other two pieces. Then I put it in the vise for 30 minutes and let it set.







After the glue set, two parallel sides of the stack were machined to make it easier to hold in a vise. The height
of the stack needs to be reduced to the width of the flywheel. Measure the gap between the standards and 
minus another .010 - .015. That should be a good width. Cut the stack to thickness.







With the stack being 3 pieces I removed half of what was needed to be removed from each side of the stack.
That centers the center piece in the stack and assures me that the spokes will be one solid piece with no
parting or glue line in them. I'm not sure it would make a difference as long as a good job was done with the
glue but I still avoided a possible visible line.







Find the center of the stack and setup for cutting. The vise was installed quickly and I didn't bother to indicate
the fixed jaw. The eyeball method should be more than adequate and the vise will be removed again for the next 
step. It is used for less than 15 minutes.







Load up the FlywheelSideOne code and get ready to cut. After the holes are drilled and you load your 1/8
endmill make sure it's a 1/8 shank and you have at least .750 of bit out of the mill. The first side cuts the
spokes completely thru so the bit goes .700 deep into the stack.







When you go to cut side 2 the wheel will get cut out from the stack. The big square of material will fall away
and I have no idea what will happen when it does. It could pinch the cutter and break it or who knows so what
I did was cut some slots in the band saw. Now I can predict the pieces will fall away without causing any damage.







To complete side 2 the piece needs to be rotated 180 degrees and perfectly aligned to X,Y center. I do that
by cutting a fixture. This is great if you are making more than one. 

Load a piece of Corian that is ugly or a piece you think you will never use. The Gcode will do a few things.
First it cuts a .01 deep pocket to make sure the surface the flywheel will contact is perfectly flat. Then the
Corian is cut out so the part can be fixtured, as is, right out of the vise. A boss is cut so the stack will be
perfectly aligned on center. I made the hub and this boss .004 different to allow for slightly under sized
cutters and backlash. 

Load the FlywheelFixture code and cut the fixture. Then move the table to a clear spot and tap the hole 1/4-20.







Load up the stack and bolt it down. The top surface of the stack will be Z0. X,Y should be set from making
the fixture and NEVER be changed in any way until the flywheel is completed.







Load up the FlywheelSide2 code and finish cutting out the flywheel. As expected the 4 corners fell off without
trouble. 







Drill and tap for the set screw. Ignore the drawing and tuck that hole back from the edge as far as you can.
Corian loves to crack at edges. Drill slow and clear the tip of the bit (peck) often. Same when tapping. Slow
as you go and back out often.







Put the flywheel on the crankshaft and chuck it up. Turn the OD down to finished diameter and your done.











View attachment FlywheelFixture.tap


View attachment FlywheelSide1.tap


View attachment FlywheelSide2.tap


View attachment Flywheel.pdf


----------



## stevehuckss396 (Dec 18, 2011)

I have decided to run the air to the cylinders using some fittings and a small piece of 3/16 tubing. The 3 fittings can be made from anything you have handy. 1/4 inch hex bar would make it easest.

I will post the new PDF drawing here and have replaced the old one in the earlier post.







View attachment Standards.pdf


----------



## stevehuckss396 (Dec 23, 2011)

This week is the piston and air fittings. You will need to make a pair of pistons and three air fittings. I made
my pistons from some acrylic pen blanks I had sitting here. Very simple turning here to get them to the
correct shape.







Whats nice about the pen blanks is they are square. That made it easy for me to hold the blank to mill the
tail of the piston. The hole was drilled and the piece was rotated 180 degrees and the other side was milled.
Then I took it back to the lathe and parted it off.







I'm still waiting for a length of 1/4 inch brass so the air fittings will not be covered but they are a simple turning
so I'm sure it won't be missed.


View attachment PistonFitting.pdf


----------



## stevehuckss396 (Dec 26, 2011)

I'm going to post the last piece early in the event that someone has the week off and might want to
try to make one over the holidays.


I changed up the design so the entire cylinder can be made CNC except the cylinder hole. It will still need
to be drilled and reamed. I also wanted a more modern look to go along with the more modern looking base
and standards. Glue up 3 pieces 1-1/4 X 2-1/2 long in the vise and let them set for 30 minutes. This code
will handle a 2-3/4 X 1-1/2 stack. I also tried to cut the entire stack away in the roughing stage so cutting
slots like the flywheel to control the scrap wont be nessessary. When ready, mill the stack to a thickness
of 1.188 inches.







Load the CylinderBottom program. Center of the stack is X0,Y0 and top surface is Z0. The program will center
drill and drill 2 holes. The hole closest to center should be tapped #8-32 before moving on. Use a bottom tap
and get as much thread as you can in there. 







After threading the 1/8 inch endmill is loaded and the bottom of the part is cut to completion. Make sure your
endmill measures .125. I have purchased cheaper endmills that were as small as .122. Not a big deal when
milling in manual mode but when in a CNC machine you can see where a circle will be .006 to big.






Now check the diameter of the 1/2 inch long shaft sticking out of the bottom of the cylinder. If it will not fit
into the hole in the standard, there are a few things you can do. You can get into cutter compinsation using
Mach3 but this is supposed to get the newer folks cutting. Mine were to big to sand or file so I went to the
next size drill and redrilled my standards.


The shaft is then cut to a length that equals the thickness of the standard. If you miss, make it a bit shorter
rather than longer. Dont want the shaft sticking out the other end.







This part is made using a fixture like the flywheel. I forgot to get a shot of the fixture but it a simple corian
fixture with a hole in it. When making the fixture I had to use the same drill bit that I used to redrill the
standards. Things like under sized cutters and backlast can have an effect on how the part will fixture so
be aware. The part is set into the fixture and secured with a single screw from the bottom.







The ball end mill is the only tool needed to cut the top. Load the CylinderTop program and touch off the top
of stock to zero Z. Like the flywheel, do not change or zero X and Y axis. I made the code for this side less
agressive because the part will be held in the fixture by only one screw. It will take longer to cut but
increase the odds of nothing bad happening while cutting.







After all the cylinders you are making are cut, use the fixture to hold the cylinders to drill and ream the 1/2
inch hole for the piston.











That's all you need to build the engine. When you assemble the engine be sure not to over tighten the screws
that hold the cylinders onto the standard. Use a real light oil to lube everything. The only 3/16 ID tubing I
could find was 5/16 OD but it doesn't look to bad. Make sure the engine turns freely and put a little air to it!

Hopefully this exercise has taken the mystery out of setting up to cut a piece and was of doing simple setups
to speed up making multiple pieces. If you have a CNC mill but have not run it in automatic, download the
code, get a few pieces of corian, go out in the shop and break some bits! Once you get going the errors become
few and far between and it keeps getting easier.


Here is a video running slow on less than 1 pound of air.

[ame]http://www.youtube.com/watch?v=f2uGxEHwLsI[/ame]


This thing flies on just 4 pounds of air.

[ame]http://www.youtube.com/watch?v=99_zorw5Zjg[/ame]




Cheers!!

Steve! 




View attachment CylinderBottom.tap


View attachment CylinderFixture.tap


View attachment Cylinder.pdf


View attachment DoubleCylinder2impTop.tap


----------



## Tin Falcon (Dec 26, 2011)

cool stuff steve . I need to get moving on this. 
Tin


----------



## stevehuckss396 (Dec 26, 2011)

Tin Falcon  said:
			
		

> cool stuff steve . I need to get moving on this.
> Tin




Now that the proto is done, I have 5 more going. Going to test some new code for the cylinders. I'm trying to smooth out the top. If it works well I will replace the old one.


----------



## stevehuckss396 (Dec 28, 2011)

I have replaced the cylinder Top code with this one. Not much different but will give a much improved finish at the very top. I had to do just minor hand work to get a great looking part.



View attachment DoubleCylinder2impTop.tap


----------



## stevehuckss396 (Jan 11, 2012)

I have two ready to ship to the person they were intended for. The brown one runs better than the prototype. It lopes along and the needle on the pressure guage never comes off of zero.

I put 20Lbs of air on the prototype to see if it would explode. It held together just fine. I could not blow it up.


----------



## stevehuckss396 (Jan 15, 2012)

3 more for me to keep.


----------



## gld (Apr 15, 2013)

Hey Steve--HELP


Finally got around to working on this thing.

Found a problem in the DoubleCylinder2impTop.tap file. It starts when Z changes too Z-0.060. Check the J in this line {G2 X-1.0535 Y-0.4449 I-1.4836 J874.3084} and here {G2 X0.2242 Y0.2443 I-0.3937 J-2075.7443}

and it gets worse when z goes to -0.09 {G2 X0.2294 Y0.4468 I0.3795 J-3535.6588}---{G2 X-1.0938 Y-0.4469 I-2.499 J1556.8827}

Steve:  Disregard...I've determined DeskCnc will not run this file. Doesn't recognize the G91.1 code.

  I have all the parts made except for the cylinder top profile. If you have a dxf of the cylinder,_  might be able to salvage this project_


----------



## canadianhorsepower (Apr 15, 2013)

Steve, would it be possible to have the G code in note pad format. I could use them on our Emco CNC as project for student's. Looks great and they could all have one to brag about


----------



## gld (Apr 15, 2013)

canadianhorsepower said:


> Steve, would it be possible to have the G code in note pad format. I could use them on our Emco CNC as project for student's. Looks great and they could all have one to brag about


 
LUC

The .tap file will open in note pad. You can then save with the extension you need


----------



## xpylonracer (Apr 15, 2013)

Hi Luc

How do you cope with the G02 and G03 commands on the Emco ? Do you use MFI ?

Rgds, Emgee


----------



## canadianhorsepower (Apr 15, 2013)

gld said:


> LUC
> 
> The .tap file will open in note pad. You can then save with the extension you need


  thanks Ill give that a tryThm:


----------



## canadianhorsepower (Apr 15, 2013)

xpylonracer said:


> Hi Luc
> 
> How do you cope with the G02 and G03 commands on the Emco ? Do you use MFI ?
> 
> Rgds, Emgee


 
I can only answer first part:fan: no problem with G02 or G03 as long as 
G17-G18-G19 are set accordingly

as for  MFI     :hDe: huhhhhhhth_wtf1does it mean


----------

