Intake Manifold CNC Pattern Test Cut

Discussion in 'Lost foam casting' started by Al2O3, Nov 17, 2022.

  1. Al2O3

    Al2O3 Moderator Staff Member

    I had a fella send me a CAD model of an intake manifold. I saved it as an .stl, used my CAM Program to reduce it to ¼ scale with one click, pasted it into a block, and ran one roughing (1/4” D Ball Nose) and one finish (1/8D Ball Nose) machining op. It had a pretty coarse stepover as I was trying to keep the machining time low (it was about 30 minutes). I had a little under an hour into it all from start to finish.

    My CAM program didn’t pick up the lower interior surface inside the carb plenums so the carb openings were cut full depth. That caused my collet to (barely) run into the rear of the interior of the rear carb pad because I didn’t have a long enough bit, and there were a couple funky things going on around the perimeter, but overall, the surface geometry was read and cut just fine.

    I'd have to section this into four or five pieces to machine all the interior features then reassemble into a pattern if I was actually going to cast it, but if someone was capable of delivering me a good model, it certainly makes one-off intake manifolds more practical. -Just me jack'n around. The pics are just as it came off the cnc after I removed it from the block.

    Best,
    Kelly

    IMG_0707.JPG IMG_0706.JPG IMG_0713.JPG IMG_0714.JPG
     
    Rocketman, BattyZ and Tops like this.
  2. dtsh

    dtsh Silver

    You never fail to impress.
     
  3. Al2O3

    Al2O3 Moderator Staff Member

    I'm working on a couple of full size intakes of my own design. CAD skills arent quite where they need to be yet but making progress as time permits. I'm looking forward to pouring hot metal on those!

    Best,
    Kelly
     
  4. rocco

    rocco Silver

    Looks great so far. On that type of manifold, what's your strategy for cutting in the runners? I'm guessing the foamie's going to have to be a multi piece glue up.
     
  5. Al2O3

    Al2O3 Moderator Staff Member

    On this one, since it's a single plane intake, looking in from the front end view, all of the runner centerlines reside on the same curved surface. So I'd just create that surface and use it to section the intake horinzontally into an upper and lower half, through the centerline of the circular runners, and straight through the carb plenum, so half of the runner ID and carb plenum resided in each piece. That would result in two pieces I could cut with 3-axis cnc from each side. Then just glue the two together. The thermostat/coolant tunnel would be machined from the bottom side of the bottom part and then a floor insert glued in to complete that cavity. This cavity would get special attention for packing and would be the highest risk of casting fail.

    On other intakes, I also need to make the flanges and sometimes the valley pan seperate pieces, if it's an air-gap type intake.

    It's kind of the joy of Lost Foam.....just break the part up into pieces that are easy to make and stick'em back together.

    Best,
    Kelly
     
  6. ESC

    ESC Silver

    Looking good Kelley.

    This is what it took to go "old school" on a dual plane manifold.

    PA210214.JPG

    PA210217.JPG

    PA210218.JPG

    PA210219 - Copy.JPG

    PA210225.JPG

    After this exercise I modified it to have a plenum for two Walbros, and later an open plenum for the blower motor. For this I baked in the mold and used the same follower as for the dual Walbros. I also had to change the outlet to clear the blower snout.

    blower manifold and corebox.jpg
     
    Blue427, Tobho Mott and Tops like this.
  7. Al2O3

    Al2O3 Moderator Staff Member

    ......and it certainly did yield a great result....on the intake and your entire V8.

    As interesting as they are, I don't have any plans for model engines at the moment as I'm pretty focused on the full size versions. I prefer lost foam for those larger parts but if I was to actually cast that scale intake, I think I'd print the pattern and have a go at lost PLA cast with block investment, especially for the water jacketed heads and block. I just wanted to test how easy it was to cut the pattern from the stl file I was given (and it was very easy). I only scaled it so it would have short run time. It's a little fuzzy, mostly because I was running nearly 200 in/min with a small bit but If I did a clean up pass of about .015 as the final cut, it would be pretty nice.

    I'd have to do some optimization on the CAM program for the same foam pattern of full size part. It would be 16x the surface area and take all day to run with the level of effort I put into the scale version, but with a little work I bet I could cut it 2-4hrs. However, if it was a 2-piece pattern with front and back machining, take that x4 for total pattern run time........it's coming on anther I'm working on, stay tuned.

    Best,
    Kelly
     
  8. Ted Brown

    Ted Brown Copper

    Excellent. I love doing the CNC as designing is as much fun as pouring. I am currently cutting mine with a flat 1/8" bit for roughing and finishing as I combined the code into one ".nc" file. The stepover for finishing is 10% and gives really good detail. Since I bought the $250 CNC to get my feet wet, I can't do any items taller than 1.25", so I make two "1" inch parts and glue. I plan to spring for the next step up that will do the whole 2" part at one time and not have to worry about sanding the parting lines. Yes... it does take more time than doing the manually, but I do like they are perfect (as much as my design) and I load them up and 90 minutes later, the part is ready without user intervention. I can also speed up the CNC travel since it's designed for wood, but right now I am still crawling instead of running, so taking my time.
     
  9. Al2O3

    Al2O3 Moderator Staff Member

    Like with anything there can be learning curve and experience only helps.

    For me, I certainly like the result, but not sure watching a cnc run tool paths evokes the same satifaction as a casting coming out of the sand....:). What I really like is the freedom to design a part from one's minds eye and then make it, but that has become more a matter of CAD rather than CAM skills, which for me was/is a steeper learning curve....but I'm getting there. It can depend on design complexity, but for 2D & 2.5D parts, I could have gotten by with just the CAD capabilities in my CAM software, but for 3D models with complex surfaces, interfaces, and hollows, a more full featured CAD program is a must.

    For roughing, flat bottom bits make more sense because the tool path calculations are simpler and the tool paths fewer to machine a given area so it results in faster roughing. If you're only cutting foam, the variation in roughing clearance from the resulting steps is inconsequential which can allow coarser stepover and faster roughing. You didn't say, but if you arent using ball nose bits for finish cuts, they will produce better finish, but the way the stepover is calculated (may depend on your software) is different, takes more compute time, generates more tool paths for a given area, and thus longer run times. It can also depend upon the resolution of the design geometry. Also, when I rough, I call for a flat bottom bit in the program for faster stock removal but use a ball nose when cutting so I don't have to stop for tool changes........just let it run right into the finish cut operation. It's still material rich with the ball nose and the additional kerf is inconsequential.

    If you are making small parts, the price you pay in machine time is small but surface area will increase with at least the square ^2 of the part size if not the cube ^3, and run time increases accordingly, so you'll become much more interested in this as your parts grow in size. Machining foam allows you to get away with things you could never dream of with harder materials. You can use bits that have >10x Diameter cut height, at very high speeds (often up to 180-200 in/min for me), and little sensitivity to direction of cut, meaning if you enable both regular and climb cutting in your programming, you can be cutting both down and back instead of retracting and rapids back to a start point. In the full size intake manifold in my first post, collectively these things can be the difference between days and hours of machine run time.

    Starting out with a modest machine can be a good move. If your X-Y envelope is suffient for your needs, it may make more snese to just modify your existing machine for more Z travel. One thing to keep in mind if/when you upgrade; you will typically need at least twice the Z axis stroke height as the height of stock you want to cut in order to get full height cutting bit above the stock plus clearance height. The height under gantry must be correspondingly higher than that. I've had plans to increase my Z axis from 4" to 8" for quite some time, but have found it very difficult to find suitable XPS stock great than 2" thick and even when I do, prohibitively expensive to acquire the minimum quanitity or ship it. Consequently, I've had less motivation for more Z travel and cut in sections if I need more than 2". I just havent found any method of laminating stock that produces acceptable results when cutting through a glue joint.

    I used my pin router to make patterns for a long time before the cnc. I think many dismissed the idea it was faster, but it often was/is as far as the actual machining time. For simple 2D & 2.5D parts I can program faster than making a pattern now, but it wasn't always the case. However, when you want to make changes or variations of a part, it's much easier to change a program than a hard template, and for machining, you can nest multiple copies and go do something productive as they are machined. When it comes to truly 3D and contoured surfaces, there's no comparison.....cnc all the way. There is an additional side benefit of safety. My over arm router is the most dangerous machine in my shop. My hands are never in danger on my cnc.

    Happy CNC'ing

    Best,
    Kelly
     
  10. Tops

    Tops Silver

    What are you folks using for CAD/CAM?

    I do my design work in Fusion360 from Autodesk, 3D print slicing with Cura, Inkscape and LaserGRBL (SVG-based) for the laser, and CAM for the router in MeshCAM (STL-based) w/CutViewer Mill to preview files. Machine control on the router is LinuxCNC.

    This thread got me going on a couple 3" wheels for dispensing masking tape in lost foam. Thanks to all who post here!
    tops_lostfoam1.jpg
     
  11. Al2O3

    Al2O3 Moderator Staff Member

    CAM = CamBam, CAD = Alibre Pro.

    I have the free version of Fusion 360 for both. Though its certainly capable software, I chose not to invest my time in Fusion. The uncertainty their business model creates as far as future ownership cost and ongoing access to both software and your own works was certainly a factor in that. As a causal user, that stability was imporatant as capability for me.

    Alibre Pro has all the capability I need, certainty and fixed cost of ownership. I may outgrow CamBam, but at the moment, it appears to do everything I need, and IMO, it's an incredibly good value. I've only taken a cursory look at MeshCam, but my initial brush with it and input from others whose opinion I value indicate it may offer similar value to CB.

    Best,
    Kelly
     
    Tops likes this.
  12. Ted Brown

    Ted Brown Copper

    TinkerCad
    Easel
    Candle

    This thing took off faster than I thought. I was already using Tinkercad Design for my lost 3D PLA/Wax setup and also making patterns in the sand casting, but was not that happy and I was very new to this hobby. So I already had my part made and just increased the size by 2% and imported the STL file into Easel. After getting my cutting setup done, I export the.NC file into Candle and it starts cutting (pretty simple for my first try). I know that 90% was having a project already designed and 3D printed out. The work was in Easel where you have to figure out the bits, etc which I am still exploring, but right now I have to get some parts made. My part is small (approx 5 x 5 x 2 in) and I will explore making a one-piece when I get the heat off me for making Corvair parts. I also learned to hot glue to sprue after slurry dipping as the glue became saturated and the part fell off. Hope to pour a few on Tuesday...between the day job and a new baby, time is getting very hard to come by.

    Wanting to take a second to thank everyone on this forum. I had almost given up on casting until I came across this site and gave the confidence and technical know-how to continue on.

    Ted
     
    Tops likes this.
  13. Tops

    Tops Silver

    Thanks Kelly, thanks Ted.

    I demo'd CAMBam years ago and it seemed very capable although a little more 'fiddly'. Nowadays I'd probably appreciate that more, to be able to fine tune settings. At the time I decided I wanted to rout parts versus take any extra time to build a router and do a deeper dive into CAD/CAM via shareware or freeware so I bought the router and an easy to use CAM program.

    Fusion360 can also generate CNC code, I need to explore that more too. It may close the gaps that I have with my familiar setup.

    I usually leave my CAD at 100%, make the STL file, and scale 101.5% while doing the 3D print or CNC file creation stage.

    Kelly, how would you do the pour cup on the little tape wheel design above? Foil cone or a small tin with Petrobond on top of the vibrated/compacted sand around the dipped pattern? I could see making the molded cups in the future, this one is more of a 'happening' as in I want it to happen soon :).
     
  14. Al2O3

    Al2O3 Moderator Staff Member

    The cnc code is gcode that is produced by your CAM softwares post processor. Understanding and being able to manipulate gcode is a whole other realm and beyond that your cnc controller has machine code to translate the gcode into 3D motion commands to drive your CNC's steppers/servos.

    I use 101.3%. 0.013in/inch or 1.3% is what you get if you apply the coeficient of linear thermal expansion for aluminum with the solidification temp to room temp. It's hardly worth mentioning for small parts but that difference is .020" per 10" part. My parts are often 20" long. You can easily see that position error when trying to drill a hole in the center of a cast boss. Various sources say the coeficient can vary for aluminum alloys but I've found this to be spot on for all my aluminum castings.

    I'd say a molded PB or just green sand cup in some kind of supporting case would be a slick way to go. Make a simple mold to pack the style cup you prefer.....some kind of offset cup with a weir preferably. Then seperate the spent bound sand from your LF sand when you demold.

    Best,
    Kelly
     
    Tops likes this.
  15. Tobho Mott

    Tobho Mott Gold Banner Member

    I played around with tinkercad a little. I found it much more intuitive than fusion or freecad but would love any tips you have for creating draft angles and fillets for sand casting patterns. Every way I've figured out seems like a clunky workaround. There has to be a better way to make a simple 3" disc with slight draft on the outside edge than modelling a 50 foot tall cone and chopping off the top 49' 11-3/4"... And that's the simplest example I can think of, it doesn't even have a raised border yet... And that's just a circle; more complex shapes complicates everything a whole lot more as well. Maybe I missed an easier way?

    Edit - realized after posting that this question is a little off topic for Kelly's lost foam thread, sorry. Still want to know though :D

    Jeff
     
    Last edited: Nov 21, 2022
    Tops likes this.
  16. Al2O3

    Al2O3 Moderator Staff Member


    Really, not so much. I was posting about reading a file I was given to cnc a pattern and I dont really have any intention of making a casting out of it so any discussion on cnc'ing patterns is fair play in my book. :)

    Best,
    Kelly
     
    Tops likes this.
  17. Melterskelter

    Melterskelter Gold Banner Member

    Not sure how Tinkercad works. But, I can say drafting is robustly supported in Onshape (and almost certainly Fusion, Solidworks, etc. ) True enough that Onshape and others take a lot of study/use to climb the learning curve. The payoff is also big, however. I have found CAD to be a bit addictive—-caution! ;-)

    Onshape is free if you are a home user. The free version has essentially all the features of the pro version, but the trade-off for the free version is that your work is theoretically discoverable by anyone. I say theoretically as your work is mixed in with countless other work pieces. You cannot search on an individual to find their work. If a person wanted to hide their work, simply naming it irrationally would make difficult for anyone else to find. I could have titled my angle plate “albatross,” for instance. It would populate my personal list with a thumbnail image. But someone else would find it only by stumbling upon it.
    Denis
     
  18. Al2O3

    Al2O3 Moderator Staff Member

    Alibre Pro (CAD) is great for draft......-very easy. Not sure about their lower cost "Atom" versions. Sort of ironic for me as a lost foam caster as it doesn't matter much for me but perhaps some day I'll appreciate it when I kick my lost foam addiction.

    Best,
    K
     
  19. Tops

    Tops Silver

    Thanks for the tips everyone, my parts turned out faithful to the quick-and-dirty, un-sanded, CNC-routered originals. I am starting to understand why people put wheels on the buckets... :) Old blue XPS foam and old drywall mud, shop scrap EPS for the sprue (probably 1.5 PCF) lightly attached with hot melt glue.

    tops_lostfoam2.jpg

    tops_lostfoam3.jpg
     
    Tobho Mott and Melterskelter like this.
  20. Al2O3

    Al2O3 Moderator Staff Member

    They looks good.....probably just like the pattern ;)

    Easy to sprue that way but maybe not as easy to coat and degate. Did you dip or brush coat?

    The through holes look pretty good but I usually don't put them in the pattern unless they are >>.5"D or so because the drill bits tend to wander and if there is any imbedded sand.......it's tough on bits. If you are going to bore them on lathe or mill it doesnt matter much other than potential for imbedded sand.

    Isn't it great to being able to put metal where you want it?

    Best,
    Kelly
     
    Tops likes this.

Share This Page