I wanted to create silicon rubber corner pads for a glass plate on which specimens will be placed. These pads will decrease the shaking that is possibly produced from the motors at the base.
I began by designing the part in Autodesk Inventor. Started by creating a 30mm cube by creating a square in a 2D sketch and extruding it by 30mm.
Then created a sketch on the top surface of that cube and drew a smaller square and offsetted it from the back face of the cube by 5mm.
Then extruded that square downwards with a cut operation by 25mm.
Then created a sketch at one side of the cube and drew an arc with a 25mm diameter and closed the loop by drawing two lines to close the corner and then extruded it with a cut operation.
But then I found out that I wouldn't have much of a base to hold the glass so I edited the sketch to decrease the diameter of the arc to 15mm.
I repeated the same process for the other side.
I then created a sketch on the bottom surface to create small parallel pads. I started by creating a rectangle with a 2mm height.
I then created a rectanglar pattern down the X direction then extruded thoses rectangles by 2 mm.
Now that I've decided that I will be milling the mould using "0.1250" DIA 4FL SE LONG AlTiN 1/8" end-mill, I wanted to redesign the part to be match the end-mill dimensions and be milled accurately.
I removed all the feature except the first extrusion and edited the dimensions .
I played around with the dimension to find the proper one to accommodate the movement of the end-mill and the desired geometry so I mad it 6 times the diameter of the end-mill "0.1250 inch" and extruded the sketch by the same dimension.
I then made a sketch on the front surface of the cube and offsetted by 1/8" from the left and bottom sides.
I then extruded this square with a cut operation leaving a 1/8" from the back surface by choosing to measure the distance between the from and back surfaces and subtracting 1/8".
Then on the bottom surface, I created a sketch and drew two rectangles on both ends on the sketch, set their heights to 1/8" and extruded them by 1/8" also.
And to make the legs completely round, I chose the fillet tool, selected the four edges of the legs and set the radius to 1/8".
And to create the third leg I created a sketch on the surface between the other 2 legs and repeated the same process.
Then on the inner back surface, I created a sketch on which I draw an arc and made it 2/3 of that surface width and then extruded with a cut operation and repeated the same process for the other surface.
The final part:
To create the negative mold for the part, I started a sketch at the bottom surface and created a rectangle around the surface and offsetted it by 1/8"
Then extruded that the resulting face by measuring the distance to the uppe face and adding 1/8" and selecting to extrude as a new solid
Then using the combine tool, I subtracted the new solid from the original part solid which resulted in the creation of the mold solid
I then figured that I should add more fillets to accommodate the endmill width; So, I suppressed The last two features (combine and extrude) to reveal the original solid and add 1/8" fillets.
Here I found that the walls should be thicker to accommodate another fillet so I edited the relevant sketch to be offsetted by "1/8inch * 2"
Also edited the extruded cut.
Then added the last fillets
Then ended up with a fitting path for the endmill
Previously, I used Modela Player to create molds but now I wanted to try Inventor HSM so I thought I give it a try; I used it in the computer-controlled machining for 2D milling and now it's time to try it for 3D milling.
To begin planning for the tool path, I had to create a library for the end-mills I will be using.
I started from the Fab Inventory sheet to look for the 1/8" end-mills.
Then by searching Carbide Depot website for "CU 130051" item number I was able to find the page of the product containing the dimensions for the end-mill.
In "Tool Library", I created a new library and called it "Fab". Hopefully this will collect all the tools included in the inventory.
Then created a "New Mill Tool" and entered that data from the website.
Note: I should have changed material to be Carbide
To get the feedrates to add them to the end-mill, I opened Modela Player and got the values from Options->Register Cutting Parameters
I then converted the values from mm/sec to inch/min. and transfered those values from the finishing parameters.
I then added the "long" variant.I used this to ensure a sufficient depth is reached
In the Lab we had a good stock of Chemical Wood (polyurethane boards).
The board I wanted to use had some holes in it so it should need some surfacing first.
I fixed the board with double side tape on the sacrificial bed.
Then inserted the 1/8" long end-mill and zeroed it on top of the board
I started setting the stock settings in Inventor HSM by clicking the "Setup" button
Then to choose the correct orientation; from Work Coordinates System I chose Select X & Y axis
I then clicked on the "X axis" icon and chose the lowermost edge of the upper surface and clicked on the "Y axis" icon and chose the left edge of the upper surface.
As I wanted to begin working from the lower left corner; I checked "Flip X axis" and selected the lower left stock.point of the upper surface
I then switched to the "Stock" tab to modify the dimensions of the stock I will be using. I changed the "Mode" from "Relative size box" to "Fixed size box" and modified the dimensions.
I started the first milling operation to be a facing so I clicked on "Face" from "2D Milling" operations.
I chose the 1/8" long end-mill and set the cutting speeds (cutting,lead-in,ramp and plunge) to be 300 mm/min
I set the speed to be 400 mm/min on a previous trial but it was too much and the machine stalled.
From the "Geometry" tab, I clicked on the "Stock selection" icon and selected the top surface.
On the "Heights" tab, I chose the "Top Height" to be "Stock top" and the "Bottom Height" to be "Bottom Height" to be "Model top". This way the facing operation will remove the 1mm space I addedas an offset for the model
To remove most of the material, I performed a "3D Adaptive" operation. I set the same speeds and tool
I then chose the downward face as a geometry.
From "Heights", I chose the bottom surface to be the bottom height so that the operation ends there.
I then set the "Maximum Roughing Stepdown" to be 10mm
When I used this value, The load on the end-mill was significant and it made horrible noise.
I let it machine a bit but then I sopped it.
So, I changed the value to be 2mm
The downward surface needed finishing so I made a "Parallel" operation to mill along the direction of its descent.
I set the parameters as I did before
I then set the "Stepover" value to be 0.1mm to increase the passes count.
Inventor HSM can export RML code for Modela MDX-20 and can connect to it serially.
I clicked on "Post Process" to convert the toolpaths into RML code.
To setup HSM to communicate with the machine I had to setup the connection first.
After exporting the file, the code editor opened and from it I clicked on "DNC Setup".
I chose "Machine 1" and clicked Setup to change its settings. I copied the port settings from the Modela Setup progrma into HSM.
Then to begin I clicked "Send" from "Transmission" toolbar to send the contents to the machine.
The process took about 22 minutes.
There was left failed toolpath from the last failed trial so I restarted the job but plunged the end-mill a little down the Z-axis
I wanted to cast silicon rubber into the mold so first I added a layer of dish washing liquid as a release agent.
I then mixed the silicon rubber with its hardener and casted it into the mold.
I left it overnight and then grabbed the casted part from the parts that were casted into the faced operation.
The most dependent corners were rounded not sharp like the mold most probably because the dish washing liquid accumulated there.