Ever wanted to put a Center Mark on an Isometric view in a drawing ?
You can’t do it with the regular “Center Mark” tool, but the video below shows a pretty good solution…
VIDEO — ISO CENTER MARK .mp4
And here is the .sldblk file I created… ISO CENTER MARK .sldblk
In my opinion, one of the most underutilized tools in SolidWorks Simulation is the Design Study. Design studies allow you to easily set up a number of ‘what if’ scenarios and run them all with the click of a button. Sure, it might take a couple extra minutes to set up a few parameters, but the extra setup time will pay off handsomely later.
Let’s take a look at the effects of varying mesh size for a stress concentration. The first step is to create and run a Simulation Study to verify the model setup and boundary conditions. Second, set up a parameter for the global element size. Third, create a design study, using that parameter as a variable. Finally, add a constraint; in this case we’ll use the maximum stress from the Simulation study we previously created. When these steps are complete, run the design study and all of the scenarios with the click of a button!
Setting up a Parameter can be done in (at least) two ways. From the Evaluation tab of your Command Manager, you can left-click the down arrow on the Design Study icon and choose ‘Parameters’. Alternately, from your Simulation feature tree, you can right-click on “Parameters” and choose ‘Edit/Define…’. The keys to creating a Parameter are to provide a name, choose the appropriate category, then link that parameter to the item you want to vary in the design study. In this example, I want to link the Parameter to ‘Global Element’ size, so I’ll click on the Mesh icon from my Simulation study feature tree.
The next step is to insert a Design Study into your model. Use the down-arrows to add the Element Size variable to the Design Study. In the second column, I chose to use discrete values for element size. These can be typed in using a comma to separate values. In the Constraints section, use the pull-down menu to add a Simulation Data Sensor to the model, specifically to monitor the maximum stress. Be sure to choose the Simulation study you want the sensor to reference for data. Then un-check the ‘Optimization’ box and click ‘Run’.
When the Design Study is finished running all of the scenarios, you will have a plot for each constraint utilized. In the picture below, the stress plot from one of the scenarios is shown. I’ve also added a ‘Local Trend Graph‘ to show the stress concentration model does, indeed, show a diverging solution with regards to stress.
I could have arrived at the same information in a couple of ways not utilizing a Design Study. The most common method I encounter is a user creating ten Simulation studies, then manually meshing each with a different Global Element size. That is, quite simply, a waste of time! The extra few minutes spent creating Parameters and properly defining a Design Study can be done much faster than creating several individual studies. I’m certain with a little investigation you can find plenty of uses for this powerful tool. Now go make your products better with SolidWorks Simulation!
This is a follow-up post to a question that I was asked recently about THIS blog entry: http://www.3dvision.com/wordpress/2012/04/14/strengthening-ribs-in-sheetmetal-new-in-sw2012/
The question was basically “HOW do I MAKE a rib like that ?”
Easy !
Start out with this:
Then create your “Rib TOOL” as a separate BODY in the file…
Then you can use the INSERT–FEATURES–INDENT command to use that “Rib Tool” body to create the indentation in the sheet metal part.
You will then of course want to do a DELETE BODY on the Rib Tool body (just select the body in the tree and hit Delete on the keyboard), and then add any fillets (don’t forget both sides) if you want them to make it look something like this when finished.
Here is a link to the actual SolidWorks part file (2013 version) if you need more guidance: Sheetmetal REMOVE FACES
There you go !! Easy when you know how… 
Imagine you have a model with thousands of faces that you need to add draft, how do you select all of them?
Here is a great tip from our good friend Alin Vargatu, from Javelin. Here he shows how you can quickly select all faces on your model that need their draft modified.
I love Alin’s work. I’ve been begging him to give a little blog love to those of us who live south of the border for years. We would have done it sooner, but weren’t sure if we would be breaking any international blog smuggling laws.
I want to clear something up that is very confusing about making SUB-WELDMENTS.
I personally had swayed people away from the Sub-Weldment functionality for quite a while, because after you went to all the trouble to get all the properties you wanted in your Cut-List Items, you would lose it all when you made a sub-welment,
NO LONGER THE CASE AS OF SW2012 !!
Trust me, it DOES work, BUT it is somewhat confusing HOW to do this the CORRECT way…
The thing to remember with this is that the BODIES do NOT store any properties, only the Cut-List Item FOLDERS do.
So if you have never done an UPDATE to the cut-list first, you cannot expect the properties (that don’t exist yet) to propagate down to the sub-weldments like they are supposed to !
It sounds obvious when I explain it that way, but it was very confusing to me for a while, and I know it is still confusing to new users…
HERE are the steps TO SUCSESSFULLY MAKE A SUB-WELDMENT:
1. Go and create your weldment as normal
2. Update the cut-list
3. Ctrl+Select the BODIES you want to make into a sub-weldment (either from tree or from screen with bodies filter)
4. Rt+Clk, CREATE SUB-WELDMENT
5. Then UPDATE THE CUT-LIST AGAIN !!!
(you will end up with 3 levels in the folder which seems strange, but it DOES inherit the properties into the Sub-Weldment like it is supposed to…)
This will even take the properties with the sub-weldment if you save it out to a separate part file (using rt+clk, insert into new part on the sub-weldment), and they will be tied/related back to the original weldment file for updating !
Hope this helps !
Remember, as an alternative to actual “sub-weldments” done this way you can always just make a weldment, make another weldment, and then stick them into an assembly together. The above method just keeps it ALL in ONE multi-body weldment PART file. And NOW IT WORKS THE WAY IT SHOULD !
To review, I had 4 main design criteria for the Remote Control Hover Craft.
I proceeded forward with the design of the Hovercraft using SolidWorks 3D mechanical design software. SolidWorks allowed me to quickly develop and execute a first pass design, utilizing Multi-Body Parts, In context Assembly Modeling, Sketch Pictures, Fastening Features, Interference Detection, and several other standard options. All of this came together in an initial design that meets the above criteria.
The design started with the Top Plate part that houses the downward facing fan assembly and gives the craft its overall dimensional size. I kept the craft under the 8″ by 8″ tray size of the Stratasys UPrint 3D Printer. The part consists of multi-bodies; one for the plate and the other for the fan housing. These bodies have minimal tolerance so they are a snug fit when pressed together for final assembly. This design criteria is so that if the propeller needs to be serviced later total dis-assembly of the craft does not have to take place. Simply pull the fan unit upward out of the top plate.
Top Plate
Exploded View Front
Exploded View Back
The chassis continues with a bottom plate and separating ribs. The chassis is hollow as the air needs to fill this cavity before exiting out of the skirt. The skirt is intended to be a bicycle inner tube cut to size with holes cut around the inner bottom portion allowing the air to escape. The skirt will be held on by two fastening plates and standard hobby store machine screws.
Section View
The back cowling snaps into place with a Snap Hook. The Fastening Feature command was used to create this geometry. The Snap Hook will allow for ease of assembly, and the cowl contains a cross bar with built in motor mount sized for a 9V-11V brushed can motor. The Cowling and Top Plate will make up the mounting location for the dual rudder system. The system is driven by an S75 Nano servo available at most local hobby shops.
Cowl
The canopy will cover all of the electronics including the Receiver, two Electronic Speed Controls (ESC), And two Li-Poly 300MAH 11.1V Batteries. One ESC and battery per motor. I originally set out utilizing the Sketch Picture and Surfacing to create the canopy structure. This worked out well, however at this time I did not have the electronics in the full assembly. When trying to accommodate the electronics under the first variation of the canopy I visibly had interference. Luckily utilizing in-context editing and having a well planned design intent, the changes to the canopy allowed for an easy and quick change.
Sketch Picture
Interference Original Canopy
Receiver & ESCs
Batteries, Receiver, and ESCs
Canopy Design Change
There is still much to do with the modeling aspect, but for now I have a good working start to the project and a starting point to investigate the flow and stress characteristics of the design. The next step is to utilize Flow Simulation to verify the lift ability of the motor and propeller combination for the lift fan and the rear facing fan assembly.
Top
Front
Back
Side
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For this blog series I wanted to design something from scratch. Not necessarily a new idea but something fun and cool. My intention is to design a Remote Control Hovercraft from the ground up.
A hovercraft or air-cushion vehicle is a vehicle capable of travelling over variable surfaces, such as land and water. The hovercraft operates by forcing a high pressure of air between the bottom of the craft and the surface below. This high pressure of air lifts the vehicle upward essentially “hovering” above the ground on a cushion of air. The first practical design for hovercraft derived from several coinciding inventions in the 1950s to 1960s. They are now used throughout the world as specialized vehicles for transport and other applications.
I have specific goals in mind that I want to meet in the design and build of this project.
I am starting from just an idea, and a sketch. We will see where the design leads.
The pattern command in SolidWorks is quite helpful for making quick work of taking a feature, face or body and copying it around in order to create a patterned set of instances. But what if you want to vary the spacing of the instances or the size of the feature being copied? The image below shows the oval-shaped cut on the left side of this muffler guard being patterned down the left side of the guard. Not only is the size changing (length and width are increasing), but the spacing between each instance is changing as well.
This is new functionality in SolidWorks 2013. Simply set up the pattern like you normally would and then activate the ‘Instances to Vary’ option at the bottom of the property manager of the Pattern command. You can increment the spacing and/or the size of the feature being patterned. For incrementing the feature dimensions, select the dimensions from the graphics window. If you need to make a modification to one of the instances, select one of the instance markers, choose ‘edit instance’ and type in the specific value for that instance. This functionality also works in the circular pattern command.
The pattern command got a power upgrade in 2013! Enjoy.
Every now and again, there are interesting Engineering feats that catch my eye. I think it happens to all of us when we’re in that Internet browsing haze (or looking for interesting topics to write about)! While I played my fair share of ping pong during college, I can honestly say that my best forehand smash never resulted in breaking the sound barrier! Enter the Purdue College of Technology, some motivated doctoral students and their Supersonic Ping Pong Gun!
After watching the video a few times, I decided to attempt to recreate this virtually using SolidWorks Flow Simulation and SolidWorks Motion. There are a couple of things to note about solving a problem like this. Since SolidWorks Flow Simulation will not physically move the ping pong ball as the air strikes it, I will have to measure the force of the air acting on the ball’s surface. I’ll use that force in SolidWorks Motion later. Also, I don’t know the dimensions of the model or the flow characteristics of their system, so I’ll make a guess or three and see what happens. Finally, with all I do not know about the Supersonic Ping Pong Gun, this should be a fun exercise to see how close I can get with a few guesses.
I started by creating a model of a launcher tube, a standard ping pong ball (40mm diameter, 2.7 grams mass), and added two lids for the Flow Simulation. I set up a Flow project using air as the fluid, an Inlet Mass Flow rate of 1 kg/s and an environmental pressure outlet. I also used the High Mach Number Flow option and set up the problem as a transient analysis, analyzing flow into the launcher for 0.00015 seconds! To be honest, my initial time setting was 1/100th of a second, but that proved to be far too long to analyze the Flow model. The last steps were to add a Surface Goal for the normal force acting on the ping pong ball and use a very refined mesh to capture the flow characteristics between the ball and launcher wall.
While running the Flow study, I watched the normal force acting on the ping pong ball rise from 0.075 N at time step 0.000116 seconds to 117 N at time step .00015 seconds. This is where I have to make an assumption about the model. The ping pong ball will start moving due to the force of the air, so analyzing the model past this point isn’t adding anything to my simplified analysis. It also wouldn’t be correct as the spacing between the nozzle and ping pong ball would change, so I considered this to be a good stopping point.
With the normal force calculated, I set up a Motion Study and use that force value to motivate the ball into becoming a high velocity projectile! Since this happens very fast, I set the Motion Study properties to 10,000 frames per second and the Motion stop time to be 0.02 seconds. The setup for the force acting on the ball is done in two steps. First, at time zero, I add 117 N force acting on the ball, oriented along the axis of the tube. Second, I moved the timeline to 0.015 seconds, edited the Force and set it to 0 N. Again, I am making another assumption about the model. I don’t know exactly when or how the force will be dissipated, so decreasing the force over a period 100 times longer than the Flow study time is, in my opinion, as good a place to start as any.
Once the Motion Study is calculated, I created a result plot of the velocity of the ping pong ball. The speed of sound is 343.2 m/s, so that is ultimately the number I am looking for. My Motion study result shows the ping pong ball reaches a maximum velocity of 325 m/s. All things considered, not too bad of a result given all the assumptions I made about the Supersonic Ping Pong Gun!
The next time you come across a really cool Engineering feat, take a few minutes to consider how you could utilize SolidWorks Simulation to prove out the results. With a few assumptions, I’m certain you could get your answers close to reality. Now go make your products better with SolidWorks Simulation!
*Disclaimer: No ping pong balls were destroyed as a result of writing this!
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