10. Molding and casting

Week 9 - 3/23/22

This week we worked on machining molds and using them to make castings.

A couple of ideas to start with.

I was actually wanting to make some silicone cast parts a few months ago, but I had forgotten about them until just the other way when thinking about what to make for this project.

I’m going to make a casting that requires a 3 part mold.

I’m going to make a little pouch for a knife.

This was the third idea I had. The first was a model of a toy, that I had previously 3d scanned in Week 5

The second was a cover for a micrometer.

However, I kept the work from these other two projects here, as I feel like it does a good job of explaining many of the techniques I went through, even if I didn’t necessarily use them for the final part I designed, machined and cast. And frankly, I think there’s a lot of good information here.

Working with 3d scans and models.

The 3d scan of the micrometer only focused on the main body. I wasn’t interested in getting a full 360 precise scan. However, one of my earlier tests of the scan (that you can see here in Week 6 ) was a plastic toy called a dunny. I’m going to use this as a example of going through the process of cleaning up the model. (Some of these techniques don’t apply to the micrometer scan, and some I learned later when prepping the dunny. And I think it provides a nicer example with a better finished part.)

Prepping the Model using … A slicer???

I had saved my models as .STL files. There are a lot of reasons not to like .STL files, however, they are common, supported by just about every piece of 3d software, and are easy to transfer the files between different software. I tend to save my files as .STLs for this reason. If your files are not saved as .STL’s, the following may not apply.

While most people wouldn’t think of using 3d printing slicer software as a starting point for cleaning up models, it’s a pretty good place to start for 2 reasons. 1) It let’s you easily orient your model in space, and gives you a reference and origin position. 2) It has access to mesh repair tools that work very well.

I used Prusa Slicer to do the following.

First I oriented the part. When you pull the part into Prusa, it may be in an odd position. I like to orient it to be in a position to be make it easier to manipulate in other CAD/CAM software.

You can use the “Place on Face” tool to help orinet the model. This tool doesn’t always work, and it may not work perfectly. However, it gives you a quick and easy starting point.

Simply choose this tool, and then click on one of the white surfaces that appear on the model to have that selected face to lay flat on the surface of the grid.

Here I’ve done this, and already this model is now easier to work with and align in other software.

Next I had a model that was full of holes, a few extra triangles, and other issues caused by 3d scans. You can see some of the issues in these images. The darker areas are main small holes.

Prusa has already fixed some of the issues with this model as soon as I imported it, but there are still many issues with this model as seen here:

But one of the cool things about Prusa Slicer is that it has a built in “Fix through Netfabb” option. Right click on the Model, and then choose this option. It may take a few minutes, depending on how large, and how many errors exist on the model.

And as you can see below, all the holes have been closed, and Prusa now reports that there are no errors in the model. This doesn’t mean that the model is perfect. But now it’s at least watertight, and many of the common errors have been eliminated.

The whole process of orienting and using Netfabb through Prusa just takes a couple of minutes, and saves a lot of time in other software.

Preparing for CAM

CAM is Computer Assisted Machining/Manufacturing, very similiar to CAD, Computer Assisted Design. And while the two are different, they’re similiar in many ways, and more and more software is capable of doing both.

I’ll be using Fusion 360 for the CAD and CAM for this part. I won’t be going over some of the basic modelling aspects of Fusion360 because that’s covered in other weeks and other users (especially on Youtube have done a much better job of showing you what to do than I can.)

First I create a new document, and then we can import a Mesh (STL) into Fusion360

While this model has been “fixed” there are still details and some problems (especially with small triangles). You can see how excellent the 3d scanner did with picking up all the small details. However, I don’t want these details. And I still want a cleaner mesh.

I can go into the “Mesh” workspace within the Design area of Fusion 360 and this allows me to clean up my .STL file.

I can then choose the “Prepare” -> “Repair” option and this will help me make a nicer model. I chose the “Rebuild” option, which really does do a drastic rebuilding of the STL, trying to clean up the triangles.

And it did an exceptional job. You can see the before and after model side by side. Fusion did an excellent job. It essentially smoothed out the small insignificant features, but left the overall shape the same. I was very pleasantly surprised how well this worked. So often these sorts of “self-fixing” software fixes do a poor job. This was not the case.

I actually only wanted to make a mold for the head of this, so I went back into the Mesh workspace, chose “Modify” -> “Direct Edit”, which allows you to edit the actual mesh. And I selected all the body parts under the head and deleted them.

I then went back to “Prepare” -> “Repair” and chose the option for “Close Holes.”

Then I went back to the “Solids” workspace and created a new sketch, which would be the stock size that I will be milling in order to create the mold.

But I cannot do much with a mesh by itself in Fusion 360 when it comes to CAM. So back to the “Mesh” workspace. What I needed to do was to create a “solid” body from this mesh, and then I can make more changes preparing for CAM.

There are a number of options here. I selected the body and then chose Parametric Operation, the “Organic” method (because of the organic like shape of this body). Resolution by Accuracy, and High Precision and clicked Okay. This may take a few minutes to process, again, it varies by complexity of the model.

Again, surprisingly, Fusion360 did an excellent job of converting this to a solid.

Now we can go design our mold.

Designing a mold

This was going to be a fairly simple two piece mold. A front piece, and a back piece.

I had already drawn a box that represented my stock size around the head of the dunny.

Now I extruded that box to about halfway to the back of the head.

Note that I made sure that the head placement, as well as the box placement would work so that there was no underhangs, or other difficult to machine places, as well as nothing that would make it difficult to remove the final cast part. This can be a challenging part of designing a mold, and you need to pay attention to how the piece to be machined/cast will work in that regard.

I can do the exact same thing with the other side of the head. And I start the extrusion where I stopped the first box.

In this case, I also tried to make sure that the box was about evenly split equally between the two halves. Again, you have to pay attention to how this entire part will work with both machining the mold, and how the cast part will work with the mold.

After I had the two separate boxes aligned with the head how I wanted them, I performed a boolean operaiton on them. This is in the Design / Solid workspace under “Modify” -> “Combine.” Click the part you wish to affect (the target body, in this case the box) and the “tool” body, in this case the head. I suggest you click “keep tools.” Choose “CUT” and then click “ok.”

Now you should see the negative of the head in your new mold. I do the same thing with the back of the head and the back box as well. Then together, you should have two halves of the mold that will have the entire mold of the head.

Next I add features that are neccessary for a working mold, such as alignment pins, sprues and flues, and bolt holes to hold it together.

now we have a mold ready to machine!

Introduction to CAM

Moving into the “Manufacturing” area of Fusion 360, we can quickly create a program to machine this mold.

First, we need to create a new setup. Click on “Setup.” This brings up the Setup Dialog box. This setup window has three tabs. A “setup”, “stock” and “post-process.” We’ll set up the stock size first. Click on the second tab, the one that says “stock.”

Setup - stock size

It’s always easier to setup stock first, and it’s even easier if you know exactly what the stock size is that you’re going to be using. I always suggest know what you’re going to make your part out of, before you design your part. Make sure that the part you want to make wil fit on the stock you have on hand.

Here you can go with the default “Relative Size Box.” But if I know what stock I’ll be using, I always choose “Fixed Size Box” and type in the exact dimensions. And then I change any of the “Model Positions” and their “Offsets” as necessary. (For example, if I have a piece of stock that is 0.500”, but I know I want to take a face pass along the top to clean up the stock, I’ll change the Z model position to “Offset from Top (Z+)” and then change the offset value to 0.010.” This tells the CAM that when I take a face pass, it will automatically clean up that 0.010” for me.

If you don’t do this, it’s not a problem. But again, it’s up to you to remember what your stock size is, and how you programmed the part to run based off of it.

Do yourself a favor, start creating a setup sheet with the information you need to know to run your part on the mill. (for a horrible, but useful setup sheet example see Week 8 Group Project )

Setup - WCS

Now clcik on the “Setup” tab. This is very important to setup correctly. If you make a mistake here, you could crash the machine, and are very likely to ruin your part. When setting this up, it’s very helpful to have some understanding of the machine that you’ll be using, how you’ll hole the part, and how you’ll find your part’s origin position when you plan to mill it. You don’t need to know this information, but it may help you understand what you’re doing here, and avoid any mistakes later on.

The first thing we need to do is align our part with the axii that we’ll be machining them along. That is make sure that the part is facing the correct way as it would be when you put it in your mill. This is the Work Coordinate System.

In this case, the part is way off. Right now, the Z axis is facing towards the back of the part. I want to change it. For me, the easiest way is to change the WCS from “Model Orientation” (how you designed your part in Fusion360) to “Select Z axis & X axis.” I then have to select a line that is congruent with the Z axis, and do the same for the X. I select a line on the box going up.

I then select a line for the X (one going left to right as we’re looking at this image.)

However, in this case, the Z arrow is pointing down, I want to have it point up. So I check the “flip Z axis” box.

(as an aside, the mill I’ll be using, the Z arrow points to the top of the machine, the Y arrow points to the back, and X arrow points to the right. This is the same as the Right Hand Rule.)

Set our Origin to Top, Center.

Now, the arrows are all pointing in the right direction, but I want my origin to be on the top of the part, and the center of the part. You may wish to have it at another location, such as the back left side of the part. Wherever the location, you need to set it here.

I want to align the top of the stock, the top of the part with the origin, where the three X, Y, and Z arrows all converge. The part origin. This is where I choose from “Origin,” instead of using “model origin” I use “stock box point”.

And now we have the origin of our part, where we’ll set the Work Coordinate, or part zero, and can use this when we make the part in the mill.

And finally, go to the “post process” tab where we’ll be using when we “post” this program; that is turn it into g-code to be read by a machine. Let’s give this a 5 digit number (whatever you want) and a short name.

Take a Face Pass.

Next we need to create a tool path. I’m going to start with a face pass, that cleans up the top of the part. It doesn’t take much material off, just enough to give me a smooth flat surface.

Choose the “Face” option under “2D” on the main menu.

The first thing we need to do when this face toolpath window appears is to select the proper tool. I’m going to use a 2” face mill because Fusion360 already supplies it. On the left side, click on “Tutorial - Inch” and then find the “2” Face Mill,” choose the material (if aluminum, choose aluminum, etc.) and click “Select.”

Set your speeds and feeds. If you don’t know what speeds and feeds to use, talk to your Fab Lab leader, they should be able to point you in the right direction.

Setting the proper speeds and feeds is important. If you don’t know what they are, go learn, and go ask someone to help. If you don’t, there’s a high chance you’ll ruin your part and break tools.

With the face toolpath, there’s nothing else we have to do. It will select the geometry for us. We’ve already set the height when we set up our stock.

The one thing you may want to do is to make changes in the “passes” tab. I usually add about 1.6” inches (for a 3” face mill, just over half the diameter) to the to the “Pass Extension” box in order to have the tool pass over the entire part (it gives a better finish with the facemills I use.)

But you don’t need to do that, and you can hit “OK.” And you’ve got a facing toolpath.

To see what it looks like, you can simulate it. Right click on the toolpath, and select simulate. Then click the play button on the bottom of the screen. You have different options to see what your stock looks like. Play around with it. When you’re done, just click “close.”

Next Toolpath - Adaptive

The next tool we’re going to use is an Adaptive 3d toolpath. This toolpath does a lot of work for us, and we just need to make sure that we tell it where to go, how fast to go, and how much stock to leave behind.

I’ll be using a 1/4” (0.250” or 6.35mm) 3 flute, square end high speed steel end mill for this toolpath.

It needs at least a 0.50” length of cut, as well as 1/4” shank (some HSS 1/4” have 3/8” shanks.)

There are a whole lot of options availabe to a 3d adaptive toolpath. And it’s beyond the scope of this to go into them all. But I’d just suggest looking at the information below and see if it can help out with what you’re doing.

Below is selecting the tool and the speeds and feeds.

Next I’m choosing where to cut. In this case I select “Silhouette” for “machining boundary” and I select the outline of the head. And for “Tool Containment” I’m using “Tool Center on Boundary” This allows the machine to just focus on this area, and not try and cut the entire part (including things like the block, and drill holes.)

Next is the “Height” tab. For this part, there’s no need to change anything here.

Then we have the “Passes” tab. There are a few things to change here. The first is to change the “optimal load.” This is how much the side of the tool will try to cut in each pass. This largely depends on the machining strategy being used and feeds and speeds. Since Adaptive toolpath is a High Speed Milling strategy, you should increase your feeds and speeds and set this to roughly 10% of your tool diameter. (In this particular case, I’ve slowed down my feeds and speeds, but I’ve increased the tool load here to compensate.)

I’ve also changed the “Maximum Roughing Stepdown.” By default, Fusion360 generally sets these very low. I’ve changed it from something like 0.060” to 0.200”. I want to rough out as much material as fast as I can.

Then you have the “Fine Stepdown” (and Fusion360 has them linked, if you change the Roughing stepdown, then it will change the fine stepdown. It’s 10% of the roughing stepdown. However, you can change this if you want a finer or rougher stepdown.) Again, this is just material removal. I want it done quickly.

And finally stock to leave. This defaults to 0.020” which is good for many things, however, for small endmills and small features, it may be too large. (or sometimes in some cases when using a square endmill and then going back to clean up with a ball nose, 0.020” isn’t enough and you’ll see traces of the square end mill in the finish.)

And finally linking parameters. You can usually leave this alone. However, if you see weird behavior, or the tool is running into stock at the beginning or end of your toolpath, this is where you can make changes to fix it.

The toolpath.

And the Simulation.

It sure seems like there’s a lot of material left. And there is. But this is where we’re going to use REST machining to remove more of the material.

I can duplicate this toolpath, change the tool to a very long 1/8” square endmill. Slow the feedrate down because it’s a fragile tool. In the “Geometry” tab, I’m going to select the checkbox for “Rest Machining” and set the “source” to “From Previous Operations.”

Then in the “Passes” tab I’m going to make sure to lower my “optimal load” (0.010” to 0.020” should work.) and change my “roughing step down” to 0.050”

This is going to take a lot more time, but at least I’ve cleared out a lot of material already. I’m being very conservative because this very long 1/8” endmill (1” LOC!) are easy to break.

Finish Milling

Finally, I’m going to copy the exact same toolpath, and change the tool to a 1/8” Ballnose. I’ll change the stepover for fine stepdown to 0.002” and and leave everything the same with the exception of “Stock to leave” which I’ll change to 0.

Change of plans, change of part.

The Knife Sock. (what’s with you and all these socks?)

The above part was for a model of a toy head. I used it to show you the process of the CAM system in Fusion 360. I did not end up making a dunny head itself (I ran out of time). But below is another piece that I created.

It’s a knife sock, a holder for a pocket knife, that will ensure it stays closed, as well as providing a lanyard hole, and also, just because.

This design required a 3 piece mold. I milled the two major parts, but I then 3d printed an internal mold part that I would to help ensure the center of this part was cast as a pocket. There is about a 0.100” (2.5mm) gap between the walls of the outside mold and the inside mold.

The mold itself is held together by 6 8-32 SHCS (Shoulder Headed Cap Screws), and I use six 1/4” dowel pins to register the two halves of the mold as well as the internal piece.

This will then have two sprues, where the silicone is poured, the part is removed, and the internal piece pulled out, and I have my part.

Design and CAM.

THe design was a simple two part mold with an inset third part that was 3d printed.

The plug

Some of the CAM toolpaths. Here you can see the adaptive toolpath to clear material from the conter, and the second image is the ballnose toolpath to provide a radius around the contour of the part.

The below are two images from the CAM. They are the same model and toolpaths, but note that for the model, I did not include any radius in the coners of the part. Instead I modelled them as sharp corners. However, if you look at the 2nd image, which is the simulating of the part in CAM, there are radiuses there.

I find it easier to simply model 90 degree corners in parts like, but just program a 1/4” (or whatever size) ball nose endmill along a contour around that wall, knowing that it will produce the 1/8” radius that I am looking for. Note that in cases like this, you need to make sure that you leave plenty of stock left on the walls and floor to allow for the radius.

A list of all the toolpaths used in both Mold Halves.

Machining

Machining Setup and Operations

For setup of the machine and running the machine, see the Week 8 Group Project which has this information. It’s a web site, use a link. I’m not repeating it here. If you would like to learn more, I highly suggest you take a Machining Operations of the Mill class at your local community college.

Haas VF1 Mill

One machine we did have access too was a Haas VF1 CNC milling center located in CPCC’s Computer Integrated Machining Lab.

Setup

Then it’s time to cut our stock, gather our tools and take it over to the machine…

We’re cutting this off of a chunk of 6061 Aluminum that is 3” x 3” x 0.5.” It’s sitting next to a 0.5” diameter, 3 flute HSS endmill.

We need a way to hold the stock, so we put it under two parallels and hold it in a vise.

When you’re starting your setup, it’s incredilby important to have a setup sheet. It doesn’t have to be professional, it doesn’t have to look nice. But you need something that has key details about the part you’re going to make, the tools you’ll make it with, and information about how you’re holding it and what machine you’ll be using.

I make a simple setup sheet. Even though it’s a decent setup sheet, looking at it now I realized he left out a key piece of information, where is the “part zero,” that is, where do I tell the machine to base all of it’s coordinates off of when it’s interacting with the stock? In this case, we went off the top, center of the stock (which on these projects is the norm for him, and he forgot to add it to the setup sheet.)

Information included in the setup sheet contains the following:

• The Part Name - “Mold Piece 1”
• The Program number - o27483
• Stock material and size: AL 6061, 3” x 3” x 0.5”
• Where the part is located from - top of stock, center of stock.
• How we’ll be holding the part - on 1 5/8” parallels in a vise
• How we hold it, ie, clearance to avoid crashing.
• What tools we’ll be using and their numbers
• T1: 3” Face Mill
• T2: 1/2”, High Speed Steel, Spot Drill.
• T3: 0.238 (Letter B) drill
• T4: #19 Drill
• T6: 1/4” HSS Ball Nose Endmill
• T7: 1/8” HSS Ball Nose Endmill
• T8: 1/4” HSS Square Endmill, 0.5” LOC
• T9: 1/4” chucking reamer
• The above also includes the length of the tools (in this case, a negative number from the Z zero position of the machine.)
• and the “G54,” the location of where the part is located in relation to the machine.
• And any notes that I take before, during or after I make the part.

Setting X, Y part location and tool touchoffs

Next we need to tell the machine where that part zero is. The X and Y location that we’ll be basing all the machine movements off of.

We used an edge finder to touch the side of the stock. In the case of going off the center of stock, we can touch each side in both axes (X and Y) and just divide by two to get the center.

Once we’ve figured out where these locations are, we enter them into the machines controller.

Next we need to tell the machine the length of our tools in relation to where the top of the stock is. This is the tool touchoff.

Here we’re using a “1-2-3” block (it’s a precision piece of steel ground to have dimensions of 1 inch by 2 inches, by 3 inches) placed on top of the aluminum stock to help touch off.

But we don’t bring the tool down to the 123 block. The block is hardened steel, it will break the tool.

Instead, with the 123 block out of the way, we move the tool down closer to the aluminum, and then while putting very gentle pressure on the 123 block, pushing it against the tool, we slowly raise the tool. And when the 123 block slips underneath the tool, then we know we’re 1 inch above the part.

We don’t want to forget to account for this 1 inch when we’re getting ready to cut. But for now, we can leave it, and that way when we can test the part in air to make sure it doesn’t behave in unexpected ways.

Later on, remember to add this 1 inch to your tool height offset.

Cutting

We have a video, it’ll be uploaded soon.

Milled Parts

Here you can see one of the mold pieces after it’s finished machining with a 3d printed inner mold part sitting next to it. All in all, I’m pretty happy with it.

Here that same inner mold piece is sitting in the part. I’m checking for fitment. Always check your part in situ. DO NOT TAKE IT OUT OF THE VISE TO CHECK THE DIMENSIONS. If anything is wrong, there’s at least some possibility of fixing it. Even if we managed to take it out and put back in, and setup our X and Y zero’s, the liklihood of it being perfect within 0.0002” is unlikely (and hey, tenths matter.)

But here, everything looked fine, and so I was able to pull the part out and start machining the second half.

The second half of the mold is just a mirror image of the first. The only real changes I made to it were switching a #19 drill used for clearance of the through hold for bolt access to a #29 drill that was used to tap the hole for a 8-32 SHCS. This was what we used to connect the two halves together.

Speeds and Feeds - I don’t know, whatever Fusion360 recommended. Feeds and Speeds aren’t that important. Don’t listen to the middle school science teacher. Look through the g-code if you care.

This is my setup sheet after I had machined both pieces. You can see all of the notes that I had written while I was machining.

Some of the notes pertained to changes to the program I wanted to make. Some of them were simply reminders so I didn’t do something vitally important when I started machining the second half of the mold (which is very similiar, but I changed out the drill bits to have one as a through hole, and one drilled smaller to be tapped 8-32.

The other information included in the setup sheet is information about offsets and any changes that I’ve made to the offsets. I had to adjust offsets in order to both make the width of the part correct to fit the 3d printed inner mold piece, as well as the depth to set the depth of the entire mold correctly, as well as to match the ball nose endmills height to the ball nose endmill height of the square endmill (to have almost zero difference and have a smooth mold.)

The setup sheet also contains notes about line numbers (N15015 for example). When I change offsets, I don’t want to have to re-run the entire program, and I don’t want to have to go to the computer and re-post everything. Instead I just write down the start line of whichever operations I think I’ll have to go back too, and I can search and find the lines, and since I’m using a post-processing option called “Safe Start all Operations” which includes an M1 and typical G90 G54 X0 Y0” and other safe-start information, I can start safely from this point and move forward.

This setup sheet has most of the information I would need to repeat the process of machining the part if I need too.)

I’m spending a lot of time talking about simple documentation. Yes, it’s that important.

Prep and Pouring

For more information on casting silicon, please see the Week 10 Group Project

While at Reynolds Adavanced Materials, we asked the salesmen, who for the tenth time was incredibly helpful, about using 3d printing and casting. And while he had been asked this question a few million times by now, I’m sure, he had good information on using Resin printed parts and silicone.

His recommendation was to use an acrylic based sealer to seal the parts. This should help with the casting and mold release. We used this Acrylic sealer here. I could not find an MSDS sheet on the material on the manufactueres website, and I’ve emailed them asking for one, but I’ve yet to hear back.

The mold released we used was the Ease Release 200 and the SDS for this material can be found here: https://www.smooth-on.com/msds/files/ER200.pdf

I sprayed one thin coat on, and then about 5 minutes before I planned to pour the silicone, right before I started mixing it, I would give it another thin coating.

I also learned a lot at this site, especially about mixing resin prints with silicone. This is where I learned that we needed to use platinum silicone rather than tin silicone to get good results. https://blog.honzamrazek.cz/2021/08/a-better-way-of-making-silicone-components-using-a-resin-printer-injection-molding-for-less-than-50-usd/

Here are all the parts for putting the mold together. And you can see the process of assembling the mold. Simply put the internal piece in, place 4 reference dowel pins around the outside, and one through the internal mold piece, put the two halves together, insert the last dowel pin, screw it togehter.

Prep

It was difficult to document the mixing and pouring process as it’s messy, I’m wearing nitrile gloves, and I don’t want to get the nasty resin on everything, so here are some images of the final poured part.

I tried two silicone mixtures. The first was Smooth-On Mold Star 16 Fast.

The SDS for this material can be found here: https://www.smooth-on.com/msds/files/BD_DS_Eco_Equ_EZB_EZS_Psy_MS_OOMOO_Reb_ST_SS_Soma_Sol_Sorta.pdf

This is a two part system. It is a 1 to 1 by Volume mixture, that has a pot life of 6 minutes, and a cure time of about 30 minutes. It has a fairly low viscosity and poured easily.

It’s a mixture that appears blueish in color.

Again it was a 1 to 1 mixture, by volume. We eyeballed the measurement by level, and poured as close to an equal amount of part A and part B in two different cups.

While it probably was not necessary, we pre-mixed both the A and the B liquid. This pre-mixing was designed to make sure that there was no seperation of the chemicals in each set. It was recommended to do this if necessary by the Reynolds salesman, especially if these bottles sit for a long amount of time. (and by the way, keep these stored in a dry, moderate temperature location.)

(These are pictures of Cori mixing and pouring from the group project. I included them here to have some type of visual representation of the mixing and pouring process, since I was unable to take photos myself.)

After the pre-mixing, we then poured the two mixtures together, making VERY sure to mix the Liquid A to Liquid B, and not vice versa, but rather to follow the Alphabet. A, B, C, D, Etc. This is a good lesson to teach pre-schoolers.

It’s important to stir horizontally, to try and limit the amount of air mixed into the material, so we won’t have many air bubbles in our finished part. It’s also important to make sure to mix the two materials thoroughly. At the same time, there is a limited pot life (the time it takes for this material to start curing) and as such, you need to be quick, but smooth and even with your mixing.

Pouring Continued

And here the parts are poured.

One thing I learned from this process is that my casting sprues weren’t large enough for thicker, more viscous silicone. Next time, I’ll try and make larger sprues. One thing that was necessary was to use a small mixing straw to force the silicone into the mold. I also had to pour very slowly to allow the silicone time to flow through the sprues. These problems became even worse when dealing with the more viscouse Dragon Skin 20 that I also poured.

With future molds, I’ve increased the size of the sprues, but also the holding capacity of the sprues, to allow for more material to sit in them, and slowly leak down into the mold.

It would also have been beneficial to have a tiny funnel to help with the pouring process.

This is the 2nd part I poured. I used a Smooth-On Dragon Skin 20 silicone product.

This product has a Shore 20A “hardness” and a pot life of 30 minutes and a 6 hour cure time. Like the above Mold-Star, it has a 1 to 1 by volume mixing ratio.

The SDS of this material can be found here: https://www.smooth-on.com/msds/files/BD_DS_Eco_Equ_EZB_EZS_Psy_MS_OOMOO_Reb_ST_SS_Soma_Sol_Sorta.pdf

One of the nice things about Dragon Skin 20 is that it has a high transparent appearance, making it ideal for coloration. We had picked up a sample pack of high visibility, UV reactive inks at Reynolds. I used the hot pink for this pour.

This product’s pot life is longer, so time is not as valuable as a commodity as mold-star’s short pot life.

I then prepared the colors. This was difficult because the color had some pigment separation. It was incredibly difficult to mix, like trying to stir a hard compacted mud in water. But you only have too add a small amount of each of the colors to the silicone, and mix it in. Tt had a large impact on the overall color.

You can find the SDS references for the colors on this page under Technical Documents: https://www.reynoldsam.com/product/silc-pig-electric-fluorescent-pigments/

Final Part

Do you see that lack of flashing? Yeah. I hit the nail on the head when it came to offsets and making sure this part was well machined. The tolerances were tight, and I hit them perfectly (just using my eyes.) Yes, I’m bragging.

Poured a number of parts with different colors

Gcode and limited STL Files

Like every other week, here are some of the files used to produce these parts. This is a limited selection of files due to file storage space. The Dunny Head alone weighs in at 5 mb.

Micsock

micsock mold 1 gcode

micsock mold 2 gcode

micsock internal mold stl

Handle Holder

Handle Holder Mold 1 gcode

Handle Holder Mold 2 gcode

Handle Holder internal mold stl

A Mic Sock.

The previous part I had been working on.

Micrometers are metrology instruments used to precisely measure parts.

Temperature has an effect on metrology. Heat (even body heat) can make metals grow, and this is the case for metrology instruments as well. This small discrepancy doesn’t usually matter, but for high accuracy machining, this could cause issues.

Some micrometers come with plastic wrapped around the main “horseshoe” that holds the anvil and thimble together. We’ve recently purchased a large number of micrometers for student usage, but they don’t have any of this plastic. I wanted a way to limit the heat transfer, but also (and really more importantly) provide a bit of protection from oils and liquids, have a non-slipper surface to grab on too, and in the worst case scenario, if someone drops a micrometer (don’t drop the mic.), it may (high unliklihood) protect the micrometer just a bit.

And so I want to make one of these.

Reverse Engineering

When I first started this project, I just used calipers to measure a micrometer, my eyes, and CAD to try and design a part that would fit around the frame of the micrometer.

I realized that I had recently acquired access too and the knowhow to use a 3d scanner, and with that…

And the accuracy is so high, that it’s easy to import into Fusion360, and then it gives me a good idea of fitment before having even to 3d print it out.

3d Test Prints for Fitment

But I’m still going to make some 3d prints just to make sure the design is correct.

First Half of Mic Sock

Other Half of Mic Sock

And the actual mold design.

The plan at the moment is to have a 3 piece mold. As it’s necessary to create a hollow style mold, I’m planning a clamshell style mold, with a semi-floating middle piece to allow for the silicone material to go around.

This was eventually changed drastically.

Molding

It came out nicely.

Group Project

You can find our group project here for now: Unit 10 Group Project

We worked on casting as a group. I helped with choosing the resins, and I like to think I provided moral support to Cori as she did most of the work of the actual mixing and pouring of the resins.

Some of the things I learned is that casting is a messy process. And it helps to have the right equipment.

I also learned that you shouldn’t lick the spatula you used to mix with, even if it does look a lot like a rainbow cake frosting.

And frankly, while messy, it wasn’t that difficult. You have to pay attention to the materials you’re working with, and pay attention to their MSDS, but that’s no different than just about any other time you’re messing with a variety of chemicals.

But the Smooth-On material we worked with was fairly easy. And I think if we had access to a vaccuum chamber, we could have gotten even better results.

It would have been interesting if we did more casting without having to machine a mold. I think I would have spent a lot more time casting, and a lot less time designing and machining molds.

References and Resources

I came across this site years ago. It’s always been a huge source of information and encouragement: https://lcamtuf.coredump.cx/gcnc/

The guy at Reynolds Advanced Manufacturing. I didn’t catch his name, but he was a wealth of knowledge and gave us a lot of information.

The machining faculty at Central Piedmont Community College, for if you want to know how to do something, just ask them.

Bonus

Bouncy Ball (left over silicone resin poured into test pieces from classifying our 3d printer. )

And a part that Cori wanted to make.

---

Last update: April 4, 2022