Have you ever broken one small feature of a part like a tab, or a flap and later found that the whole component is useless without it? Well, that’s what happened to me with my portable water distiller. I dropped the small plastic lid that holds the collection canister in place and it exploded on impact.
After a cursing the materials and design for not being able to withstand a six-foot fall, I went to the manufacturer’s website to find out how to order another. Finding my way through the labyrinth that some web pages can be, I found the parts list for my water distiller; the one part I need to order, of course, is a non-orderable part. The cynic in me immediately jumped to the conclusion that this was a planned design flaw. I then thought to myself “Hey, I have SolidWorks. Why don’t I design a better lid and ensure that it can withstand a drop test while I’m at it.” So I did just that.
After gathering the broken shards of the lid, I grabbed my ruler and started taking measurements. In hindsight, I should have used a more accurate measuring tool but that is a whole other story. With my dimensions in hand, I went into SolidWorks and began my design. My first idea was to reconstruct an exact copy then make some changed to improve the design. Looking at the broken piece I recovered I realized that the lid and flap were two separate parts, and I noticed that there were tiny little plastic tabs holding the two pieces together. At that point, I decided to scrap the original design and make my own.
Since I was planning on 3D printing parts on a Projet 3600, I designed the lid as one piece with the hinge for the flap inlaid into the lid itself. This way there is no need for assembly, and another potential failure. I used the following design constraints to ensure that my 3D printing parts could be created:
Minimum thickness – 3 mm
Tolerance for moving components – 0.054 micrometers
A minimum thickness of 3 mm was recommended by the Digital Manufacturing Lab to ensure the part was strong enough for the use I needed it for. This thickness was very easy to design in SolidWorks using the shell feature.
In order to have the clearance to move the parts but have a tight enough fit so the moving components do not wiggle and bash about, I was told to give a clearance of 2X the printing resolution of the machine (UHD was used with a resolution of 29 microns). This ended up being 58 micrometers. I used that clearance on the cylindrical hinge of the flap, as well as the side clearance for the flap. To capture this design intent, I used a top-down design method so I could relate the flap to the lid and ensure the 58 micrometers was met everywhere on the part. While in a sketch of the flap part, inside an assembly, I used the offset entities command to create the geometry of the flap using the external geometry of the lid. To capture the clearance in the other dimension I extruded this sketch with an offset from surface end condition.
I could have made this as a multibody part and captured the same design intent, but in a multibody part, the components would not have moved relative to each other like they can in an assembly. If I would have made the lid as a multibody part I could create an assembly from it by saving the multibody externally as derived parts. The next step would be to create an assembly, but use the original multibody part as an enveloped master model so the derived parts would automatically line up when they are inserted into the model. There is no incorrect way to model a part but I chose to use the top down assembly approach for this example.
After the assembly was complete I wanted to make sure my design intent was captured successfully so I used some of the tools in the evaluate section of the command manager. To ensure that my part had the desired thickness of 3 mm I used the Thickness Analysis tool. The tool is very simple to use to detect values above or below the desired thickness, but can only be used on a part file so I had to check each component individually. I chose to show the regions thinner than 3 mm and the results are displayed below.
It’s safe to say I call this a success. There are two areas that gradually lose thickness and that’s because they are a corner. As the flat face gets closer to the outer edge the distance between the two gets narrower, as shown in the pictures below. I could thicken the whole part to make this thickness 3 mm but I don’t think that is necessary. I will let the drop test and human handling analysis determine if stress will concentrate in this area and cause failure.
To ensure that my desired tolerance was modeled correctly I used the Clearance Verification tool in the evaluate command manager of an assembly file. By setting the minimum acceptable clearance to 0.054 mm and choosing to check the clearance between the two components, the calculation took no time at all and resulted in no clearances below the set value.
When selecting the material I had a few criteria in mind to help me determine the material. Some of the major concerns were human exposure as I will be handling the object regularly. Water safety and solubility were also factors as it will be in close proximity to my drinking water. Additional concerns included strength, and of course cost. To gauge the material I downloaded the Safety Data Sheet and had a read. The structural components of the material seemed perfect, and the cost was within budget but the toxicological information made me a little leery. Since the material is UV cured it is also UV sensitive so I will coat the part with a nontoxic spray which will solve both of my concerns.
I have included the worst case scenario I could think of for the drop test. The simulation has the lid falling open and impacting the floor from a height of 6 ft. The stress accumulated from the impact exceeds the yield strength of the material but only in the area of impact. The stress that propagates through the part is far below the plastic deformation range so I feel that the part will survive a drop with only minor damage to non-crucial geometry.
I ran a static simulation to see how the part could withstand human handling. My goal was to see how much force was necessary to break the lid off. After some mesh refinement, I ran a simple static analysis to better understand the lid I had created. The final results pointed toward plastic deformation occurring after about 2.5 N of applied force when set up like the picture to the right. After a bit of research, I discovered that the average person could put about 80 N of force with just their fingers. So if I wanted to I could break the part with one hand and after testing this theory on my pen I was surprised at the power of one hand. Not to brag about my strength but I snapped this pen by gripping it between my fingers and pressing it forward with my thumb.
After receiving my part from the printer it was absolutely perfect, it looked just like the 3D model. The flap on the lid moves smoothly without any unexpected resistance and no knocking at all. The fillet edges feel smooth and the part feels strong. I even dropped it on the same floor with no noticeable damage to the part.
I had read all the data cards on the printer and seen its resolution but I wanted to prove the accuracy of the print myself so I grabbed my Vernier Calipers and went to work taking some measurements.
The first dimension I measured was the wall thickness of the circular portion. Using the measure tool in SolidWords the wall thickness is 3 mm. The calipers verified that measurement with a measurement of 3.00 mm ± 0.02 mm.
The next measurement of interest was the internal diameter of the hole. SolidWorks dimensioned this number as 11 mm and the calipers confirmed that measurement exactly.
The external diameter of the lid was dimensioned as 45 mm by SolidWorks and the real world measurement was precisely the same.
The final measurement I decided to take was the thickness of the flap. The software and real world measurement both yielded 3 mm.
After the measurements were so accurate I decided to weigh the part to obtain the mass and compare it to the mass properties in SolidWorks. The software predicted the weight to be 14.285 g but my cheap kitchen scale weighed the printed part in at 16.1 g. This is close but the weight discrepancy could be some leftover support material caught in the internal geometry or a slight difference in mass density then input into the software. The part works perfectly for its chosen application and I am truly happy with the results
That concludes this article on 3D Printing Parts – A Real World Application. There is a myriad of other new features and enhancements not covered in this article which we will detail in later posts. Be sure to check out our Webinar Wednesdays, and keep an eye on this page for new articles on our ever expanding capabilities; SolidWorks, SolidWorks Electrical, Enterprise PDM, SolidWorks Composer, SolidWorks Plastics, SolidWorks Simulation and CAMWorks.
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