Quarter Scale V8 Engine

[Tool-n-Around]

I’m wondering whether thus is this something that could be done with the Unroll 3D Model and Wrapper plugin in CB? Is it? Having briefly looked at the documentation for those plugins it seems maybe.

I was given an amazingly complete model of an engine and have a friend that wants to make a running ¼ scale version of it and asked if I could make a set of aluminum engine castings for him. Some of you know, I use CB to make foam patterns for the lost foam casting method. Though these parts may be better suited 3D printed evaporative patterns for block investment casting, I thought I’d have a look at what I could do with how I’m presently geared. Unlike other models you usually see on Thingverse and similar sites, these models were remarkably detailed and accurate. They had some errors which I repaired and now have clean STLs. The block and cylinder heads are the two candidates. Pictures attached below with the propped 4th axis of rotation.

I quickly set up and simulated some sample programs. They were 3-axis programs of all 6 sides. With a .125” ball nose bit with .1 stepover and scanline MOPs, all sides were < 10minutes of run time, but, because of the geometry, not all of the surface could be machined in the six orthogonal runs. To provide some scale, the engine block is about 6” long.

I thought about making a small fixture to index 4/6 orthogonal runs and then just thought why not expand my horizons and try the 4th axis I originally bought with the machine to machine 100% of 4/6 orthogonal setups and then do the ends in two separate operations.

My machine controller is 4th axis capable and was delivered by the manufacturer with a proprietary version of GRBL. I have the 4th axis hardware which is a bit of a toy but should be fine for machining a small foam piece like this.

Possible? What say the CB brain trust?

Best,
Kelly

[dh42]

Hello

I’m wondering whether thus is this something that could be done with the Unroll 3D Model and Wrapper plugin in CB? Is it? Having briefly looked at the documentation for those plugins it seems maybe.

Not sure !

I think it will be better to use positional machining.

http://www.atelier-des-fougeres.fr/Cambam/Aide_V1/tutorials/Usinage4axes_EN.htm

I quickly set up and simulated some sample programs. They were 3-axis programs of all 6 sides. With a .125” ball nose bit with .1 stepover and scanline MOPs, all sides were < 10minutes of run time, but, because of the geometry, not all of the surface could be machined in the six orthogonal runs. To provide some scale, the engine block is about 6” long.

I think you need a mix of 4 axis machining and 3D machining to achieve this project.

4 axis positioning for the surfaces that must be very flat like the top of the cylinders, and 3D for the foundry areas.
 
++
David

[Bob La Londe]

Another thing to think of is setting up indexing.  I have a 4th axis, but I've made a few parts using face to face spin indexers that you would think were 4th axis machined. 

[Tool-n-Around]

Positional machining and indexing is what I was getting at in my second to last paragraph with a manual indexing fixture. Other than the 6 orthogonal views I think I could get most all of the rest with a couple additional positions and selective bounding regions. However, I suspect I might be better off 3D printing them in an evaporative pattern media for block investment casting.

The valve covers have the finest detail. I wanted to see the art of the possible with the level of detail possible for my lost foam processes. I made a quick program for my CNC Router to make a sample pattern. Each side was about 8 minutes with a .125"D ball end mill and .1 step over. I chased the ribbed and logo/lettered area with a .031"D ball end mill which barely fit the letter spacing and as you can see, did not clear all of the logo features. The result is in attached pictures.

My take: Not good enough detail. These would need to be lost resin/block investment cast probably with Zamak to get the detail. If you have to resort to < .031 cutter for detail you're probably not going to get there machining polystyrene foam.

Best,
Kelly

[Bubba]

I'm familiar with 4th axis work, and I wouldn't mess with it. Considering the time and effort required, CB and its plugins (as of now) are not capable to deliver this. A dedicated software for that kind of work would be a fine challenge.
As Bob mentioned, you can use the axis as precise indexing tool.   

[Tool-n-Around]

Haven't tackled the block and heads yet but decided to machine patterns for some of the other "easier" engine parts. Below are the front timing cover, bell housing, and oil pan shown along with the previously machined valve cover. All 2-sided machining with .125" ball end mill and .1 res and stepover, 150in/min. They are all about .090" wall. That's quite sporty and will be quite the challenge to cast.

Best,
Kelly

[EddyCurrent]

Kelly,

What is the material you are using for those patterns ?

[Tool-n-Around]

Kelly,

What is the material you are using for those patterns ?

It's extruded polystyrene foam insulation board. It's relatively inexpensive and commonly available in US home improvement stores and the density is between 1.3-1.5 lbs/ft3. It gives a nice trade-off between machinability and burning out clean for the lost foam casting process. Higher densities will machine and finish better at the expense of reduced performance for casting process.

It is a pretty good material for proving programs too. It's like cutting air except you need a good dust shoe/collection system and good grounding for your machine because the chips can generate quite the static charge and will cling to everything without.........but is also very easy to clean up with vacuum.

Best,
Kelly

[Tool-n-Around]

I made some improvements to the valve cover program last night from my arm chair.

Mostly in the logo and rib area.  I remembered I had some .5m end mills (.019") compared to the .031" EM I had been using. The graphics are so small I couldn't get the .031" tool path around all the letters.

Instead of allowing the 3D MOP to cut the artwork, I isolated and filled the graphics area by generating a patching solid in CB used along with the STL, and edge detected the graphics from the original STL so I had them as polylines.

I enlarged those graphics polylines by 10% to give me a little more operating space and then proceeded to make subtle changes to the fonts by dragging the nodes/handle on those polylines to open the pinch points and increase font width in areas where it was too thin to survive cutting.

With the graphics being polylines, I could now cut them with a pocket MOP and even with a .5mm EM the run time was only 60 seconds for the logo at 15in/min and all the speed the router had.....probably 20krpm. I could make additional drag/shape changes to the polylines without changing the pocket program, so being only 1min/cycle, I started experimenting.

After a few cuts I observed the cutting performance wasn't very repeatable and pretty quickly concluded it was due to play in my rack and pinion drive. So I tightened up the pinion clearance and it helped, but still can notice the hysteresis when it changes direction. It's probably only .002-.004" but when you apply that per side of a font that is only .020" wide at the narrows, it's significant. If I go tighter on the R&P I risk losing steps from binding. Makes me wish I converted to ball screw when I did my machine upgrades.......which I have, I just didn't make the hardware to install them......future project!!

You can see below my experimenting and two more sample pieces. On those, the font looks pretty good on the first one but was displaced off center in the rib pattern. On the next piece I moved the graphics to be centered in the ribs but the font cut smaller. I'll fiddle with it a little more. Looks like I'll have plenty of sample patterns for developing the casting 

Best,
Kelly

[dh42]

Hello

Even smaller tools exists ...

Example here with Ø 0.3mm (0.012") at affordable price (7.20€)

https://www.sorotec.de/shop/Cutting-Tools/sorotec-tools/1-8-tools/1-8--Shaft-Mill-Tools/2-Flute--Flat-/

Maybe you can ask you dental if He have some used tools for you (mine give me some)

++
David

[Tool-n-Around]

Hello

Even smaller tools exists ...

Example here with Ø 0.3mm (0.012") at affordable price (7.20€)

https://www.sorotec.de/shop/Cutting-Tools/sorotec-tools/1-8-tools/1-8--Shaft-Mill-Tools/2-Flute--Flat-/

Maybe you can ask you dental if He have some used tools for you (mine give me some)

++
David

For sure, but I can machine must smaller features than can be replicated in the foam (limited by foam cell size), or than can be practically filled in an aluminum casting process. If I was using block investment casting with vacuum or pressure assist, and a different evaporative pattern media, finer detail is possible whether machined or 3D printed.

Best,
Kelly

[lloydsp]

Even smaller tools exists ...

Example here with Ø 0.3mm (0.012") at affordable price (7.20€)
-----------------------------

David, the other problem (besides the cell size of the foam) is spindle speed.  Bits that small require IMMENSELY FAST spindles to work well.  Or, extremely slow feed rates.

If I need 20Krpm for a 3mm cutter, I can extrapolate that a 0.3mm would require 200K for the same feed rate.

When I was modeling a lot, I used to have a very old 2nd-hand air-powered dental drill that would run at over 200Krpm.  I'm sure those could be adapted to work, but I've never seen one of them mounted on a CNC machine.  I also don't have any idea what their useful duty-cycles are.

Lloyd

[Tool-n-Around]

......David, the other problem (besides the cell size of the foam) is spindle speed.  Bits that small require IMMENSELY FAST spindles to work well.  Or, extremely slow feed rates

Yes, however, my .5mm carbide bits are 4-flute so although that helps by 2x, it isn't helpful for ejecting/clearing chips. I had another iteration on the valve covers yesterday with very good results. I backed the feed down to 15in/min. With the graphics pocket MOP so short of run time, I may try 5in/min. The other issue I have is I need to use a shank extension to use this small .125" shank .5mm EM because I use other larger/longer bits in the same part machining sequence that needs more Z clearance.

I bought a 10-pak of those .5mm carbide end mills several years ago off Amazon for $15 delivered. Didnt have a need for them at the time but thought they could be handy for some work like this so I grabbed them. Don't know much about their quality, and 4-flutes isn't helpful for strength, but for cutting foam, it's not much of an issue.

A couple weeks ago during a toll change, I accidentally forgot to reduce the speed before I started up and folded one of those over. I was contained in my cast dust shoe but more way excitement than I care for. Consequently, I'm a bit sheepish about running at full speed with the .5mm bit. -But I'm getting there and am confident I'll have good enough machining results. Whether I can actually cast the fine detail I can machine may be another matter.

Best,
Kelly

[dh42]

Hello

OK, thanks for explanations ... I've no knowledge at all about casting and casting foam machining. Some years ago I have a try with "styrodur" (insulation foam) to make "tool print" for a box but it is my only experience with this kind of soft material.

https://www.youtube.com/watch?v=CArJdBT0ok8



++
David

[Tool-n-Around]

I cast a few sample valve covers. Not too bad. Still have a couple ideas for further improvement. Here's a link to a short YouTube video of the result.

https://youtu.be/IW7p5kkQhO8

Best,
Kelly