Lab 1 - Rapid prototyping I. - design
Lab 1 - Rapid prototyping I. - design
LAB: Rapid prototyping I. - design
Goal: learning how to design a microfluidic chip for 3D printing.
Tools needed: Autodesk Inventor -> see FAQ
Video tutorial:
Goal: learning how to design a microfluidic chip for 3D printing.
Tools needed: Autodesk Inventor -> see FAQ
Video tutorial:
- Not possible in MOOC version
If you would like to register and get graded for the course, please see FAQ-1.
OVERVIEW
In the rapid prototyping classes, you will gain a basic understanding, skills and knowledge necessary to design and 3D print prototypes. These are skills that you will find useful as an engineer, irrespective of your background. You will go through the computer-aided design (CAD) process of a microfluidic chip prototype in Autodesk Inventor, which then will be manufactured using a DLP/SLA 3D printer. Topics covered (Lab I):
- Use of CAD software
- Prototype design in CAD
- Preparing a prototype for 3D printing
During the design class, you will make a basic reactor chip with 2 inlets/outlets with micropillars inside the reactor. The design example is given.
REPORTING GUIDELINES
Not relevant in MOOC version.
BASIC CHIP
DESIGN TUTORIAL
REPORTING GUIDELINES
Not relevant in MOOC version.
Depending on your knowledge of a CAD software, you can do it alone or together with the practice leader. If you cannot finish on time during the lab, you can register and download the student version of Autodesk Inventor for free here. The chip design we make is typically called an H-microreactor:
(http://www.makefluidics.com/en/products/3-pack-coc-h-microreactor).
Using
Autodesk Inventor for the first time, it can be useful to go through the
tutorial(s). The toolbar called Get
Started gives you access to the Tutorial
Gallery. A quick and easy tutorial how to make your first part can be found
by typing in the search “Basic Part Modelling: Shelf Support Bracket”. For a
little more detail, search by “Fundamentals”. There are various tutorials you
can go through depending on your skill level.
DESIGN STEPS
1. Designing the base of the chip according to the specifications. Follow the guidelines below.
a. In Autodesk Inventor open a New File → Standard (mm).ipt – This is found under the Metric templates.
b. Start the 2D sketching mode from the action bar. The first sketching plane can by any of the three, in a 3D printer software, this can easily be adjusted.
c. Draw the chip’s surface LxW 75 mm x 25 mm. Use the rectangle tool from the toolbar. I suggest using the Two Point Center option.
d. Finish the sketch.
e. From the toolbar, choose Extrude and type in 1.5 mm for the thickness of the chip. To reorient the part, hold Shift and move the Middle Mouse Button.
2. Placement of the inlets/outlets. – Save your work.
a. Begin a new 2D sketch and choose the one of the larger sides of your part.
b. Choose the Circle tool and draw a 2 mm diameter circle on the chip.
c. Next, choose the Dimensions tool on the toolbar. Firstly, click on target edge of the chip, then the outline of the circle. Type in 6.5 mm. This will adjust the position as needed.
d. Since there will be an inlet or an outlet in each corner of the chip, their distance should be 6.5 mm from the closest 2 edges. Use the Dimensions tool to adjust their location.
e. Next, within each circle, draw a smaller 1.5 mm diameter circle. Use the center point of the larger circle for good allingment.
f. Stay in the Sketching mode.
3. Sketching the H-microreactor. – Save your work.
a. Use the Rectangle tool to draw a LxW 20 mm x 5 mm rectangle in the middle of the chip. This can also be seen from the annotations on Figure 1.
b. Select the Line tool from the toolbar for drawing the connective channels.
c. Starting in this example from the top left 1.5 mm diameter circle, place the first point of the Line on one side of this circle (to target convenient points, Autodesk Inventor assists with a snapping feature) and the other Line point to the top corner of the 20 mm x 5 mm rectangle. If the target does not snap to the centers of the circles, you have to use Project Geometry to get the 2mm circles from the previous sketch (Sketch 1).
d. Next, draw a second Line starting from the other side of the same circle, connecting now with the middle of the rectangle’s shorter edge.
e. Continue this pattern for all 1.5 mm circles at the remaining corners. In the end you should have the channels like they are on Figure 1.
f. Finish the Sketch.
4. Extruding the inlets and outlet features. – Save your work.
a. Use the Extrude tool, select all four 2 mm diameter circles. In case you selected an unwanted surface, hold down Ctrl and click on the part again, sometimes it takes two clicks.
b. Once all four are selected, set the distance to 6.5 mm and reverse the extrusion direction so that the hollow cylinders would be created inwards through the chip and out from the other side. Be sure that the ribbon next to the Distance editing box in the Extrude tool pop-up window has Join selected.
c. On the left of the Autodesk Inventor, you should see the Model bar, you should also see the Extrusion 1 and 2 that you’ve made so far. Click the + next to Extrusion 2 to open it and then right click Sketch 2 and click Visibility. Click again later to hide the sketch.
d. Next, choose the Extrude tool again. This time we select the 1.5 mm circles.
e. Repeat this for all four circles.
f. In the Extrude tool window, set the Extents drop-down value to “All” and click OK. This automatically sets other features to Cut and reverses the direction of the extrusion as we need.
g. Rotate the chip to check your extrusion result and compare to Figure 1. Fillets are still needed.
h. Choose the Fillet tool from the toolbar. Select all of the bottom edges of the inlets/outlets extruded features.
i. In the Fillet tool window, set the Radius to 0.5 mm and click OK.
5. Extruding the H-microreactor channels. – Save your work.
a. From the toolbar, choose Extrude and select the rectangle of the microreactor and the channels connecting to it. Make sure to also select the 2 mm circles of the inlets.
b. Set the Distance value to 0.3 mm.
c. From the left side ribbon choose the Cut action.
d. Verify the cutting direction and click OK.
6. Micropillars - Staggered cylindrical - minimal dimension of ~0.3 mm as defined under specifications in Section 1.3. – Save your work.
Figure 2: Staggered cylindrical micropillar design. (Showing also COMSOL simulated likely fluid mixing effect produced by this type of micropillar design)
a. For convenience, hide the Sketch2 as was done in step 4.c.
b. Start a 2D Sketch inside the microreactor and again draw a LxW 20 mm x 5 mm rectangle in the middle of the chip. Use the line tool to draw the center lines of the rectangle. This creates edges that we can use for easier constraining of the micropillars. The lines will snap to the centers of the edges.
c. Let us start from the middle. Let us use 0.5 mm diameter cylinders as micropillars and 0.4 mm as the minimum gap size between pillars and the walls, the maximum number of pillars in a column can be five for this case. But we will start with the shorter column with 1 less pillars in the ‘Staggered’ design.
d. Use the Circle tool to draw a 0.5 mm circle in the reactor area.
e. Use the Dimension tool to set the distance of the circle from the vertical cross line to zero.
f. Use the Dimension tool to set the distance of the center of the circle from the horizontal cross line to 0.4 mm.
g. Add a second circle above the previous, keep the distance from the vertical cross line at zero and the gap between circle outlines to 0.4 mm.
h. Next we move on to the 5-pillar column, on the right side. Draw a circle exactly on top of the horizontal line and a little bit to the right of the first drawn column.
i. Use Dimension to set the distance between the closest circles to 0.4 mm.
j. Draw 2 more circles above it and be sure that the gaps between all closest pillars is 0.4 mm. Use the Dimensions tool. When defining the dimension make sure to select the closer sides of the circles. While positioning the centers of the circles make sure they are on the same line (the center of the new circle will snap to the line if it’s moved to the correct position)
k. At this point you ought to have 5 circles positioned.
l. In the toolbar, under the Pattern section, choose Mirror. In the popup window, you should have the “Select” option already active. Drag your mouse holding the left button down over the 5 circles to select them. Dragging ought to be done from left to right to only activate lines that you’ve selected in entirety. If you have selected the center lines or diagonals, deselect them with Shift+click.
m. In the Mirror window, activate the “Mirror line” and choose the horizontal cross line and click Apply then Done.
n. In the toolbar, under Pattern section, choose Rectangular. Select all of the circles you now have.
o. In the Rectangular window under Direction 1, click on the currently inactive cursor button and select the horizontal cross line. Verify that the directional arrow is pointing to the right.
p. In the Rectangular window, under Direction 1, in the first box we write 7 as the number of repeated duplicates drawn in the desired direction. To the bottom box, write the precalculated distance of 1.558846 mm, click OK. If you have selected the center lines or diagonals, deselect them with Shift+click.
q. Open the tool Rectangular in the Pattern section again. Select the same first two columns of circles. For the Direction 1 arrow-line, select the horizontal cross line again, but this time also click the button next to the cursor button to flip the direction the duplicates will be drawn in.
r. In the numeric boxes, write the same values as before and click OK.
s. Finish the 2D Sketching mode.
t. Use the Extrude tool, select all drawn circles and set the extrusion distance to 0.3 mm. To deselect objects that you don’t want to extrude, use Shift+click. Make sure Sketch 2 is not visible during this step and deselect the rectangles, only leave the circles selected.
7. Adding engraved information onto the chip. – Save your work.
a. Turn over the chip to the extruded inlet/outlet side and start a 2D Sketch on it.
b. In the toolbar, next to the Rectangle tool, choose Text. Choose a place for your text on the surface of the chip so it wouldn’t cut into other important features.
c. Type in your initials and the date DD-MM-YYYY.
d. Select top view (the view changer is in the top right corner of your workspace window). Use the Rotate tool to rotate the text 270 degrees. As Center Point, use the center point of your design. Then drag and drop the text to the lower left corner of the chip such that it does not overlap with the inlets.
e. Finish Sketch.
f. Extrude the added text using Cut mode, inward direction and a distance of 0.5 mm.
8. Last details – Fillet the corners of the chip. – Save your work.
a. Use the Fillet tool from the toolbar, select the 4 corner edges of the chip and fillet them with a Radius of 2 mm.
9. Proceed to making your model ready for printing (Next section) – Save your work.
PREPARING DESIGN FOR 3D PRINTING
Figure 3: Example chip CAD model prepared for 3D printing. The chip will be supported on the narrow side.
To be able to 3D print your chip without typical defects which can occur at the first several layers of the print, you should design supporting columns to distance the chip from the printing platform. The recommended supports are cylindrical columns with 1 mm diameter and 10 mm of height. The chip’s footprint at the end of the support columns, should extend 1 mm beyond the chip from all sides and should be 1 mm thick. Follow the steps below:
1. Design Support columns to the narrow side of your chip (see Figure 3 above).
a. Rotate your chip, such that the long narrow side is on top and easily visible.
b. Start a 2D Sketch on it.
c. Draw a circle with a diameter of 1 mm on that side.
d. Use the Dimension tool to set the circle in the middle of the vertical axis. This can be done by knowing that the thickness of the chip is 1.5 mm, so the distance from the edge should be 0.75 mm.
e. Using Dimensions, set the distance from the center of the circle to the shorter edge of the rectangle surrounding your drawing area to 1.5 mm.
f. Using the Rectangular Pattern, select the drawn circle. For direction use the long horizontal line. Insert the values for 35 duplicates with the spacing of 2 mm. g. Finish the Sketch.
h. Use the Extrude tool. Select all drawn support column circles and extrude them by 10 mm.
2. Add the Chip’s footprint (see Figure 3 above). – Save your work.
a. Start a 2D Sketch on top of one of the support columns.
b. Use the Rectangle tool to draw a rectangle starting from the center of the middle support column. Use LxW of 77 mm x 3.5 mm. This will draw an area with each side extending 1 mm further than the chip itself.
c. Finish the Sketch.
d. Extrude the drawn surface by 1 mm.