Using a Shell Mesh with Thin Components

I’ve always been clumsy when decorating my Christmas tree, consistently working my way through my decorations at a rate of two to three baubles per year.  This inconvenience of having to replace broken baubles has taken its toll and I’ve decided to design the world first structurally sound bauble. 

How can SOLIDWORKS Simulation help? Well stage one will be to determine how much force one of these baubles will withstand before breaking, that way we will have a basis for comparison.  In order to do this we’ll set up a simple stress test to begin with, with a fixture to simulate my hand holding the top of the bauble and a force to represent the moment when I idly bump it into something and turn another shiny ornament to a glittery mess on the floor.  This is where I face problem one:

In order to achieve accurate results, it is recommended to have at least two high quality mesh elements across the thickness of your part, with our wall thickness of 1mm we therefore require an element size of 0.5mm.  This would result in an incredibly dense mesh across the surfaces of the model, which in turn would take an unreasonable amount of time to both mesh and solve for a part of this simplicity. 

We can therefore use an alternate mesh type for thinned walled parts (such as our bauble) known as a shell mesh.  By utilizing a shell mesh, it is possible to drastically reduce the mesh complexity resulting in significantly faster solve times in models which feature a thin cross section.

To define your thin walled solid bodies as shell’s follow this process:

Step 1: Right click your chosen body in the Simulation tree and select ‘Define Shell by Selected Faces’

Step 2: Select the faces you would like to define as a shell.  Also input the thickness of your material as well as the material offset to determine where the top and bottom faces lie.

Step 3: Re-mesh your model to create your shell mesh.  Ensure you remove any small element size you may have added trying to achieve two solid elements across the material thickness as these are not necessary for a shell mesh.  Once meshed you will notice both the ‘inside’ faces and ‘outside’ faces are highlighted in different colours, ensure the ‘outside’ and ‘inside’ colour is consistent and doesn’t swap between faces. 

If you have a mismatch of shell colour select the face, right click the mesh in the simulation tree and choose to ‘Flip Shell Elements’

Step 4: Run your simulation and get your results in a fraction of the time it would have taken using Solid Elements.

Whilst I continue my design quest of the unbreakable bauble (You hear it here first…) why not give shell elements a try for yourself and see how this technique could save you analysis time.

Merry Christmas from everyone at TMS CADCentre!

Generating tapped holes on non-planar (cylindrical) faces.

 

As a SOLIDWORKS Elite Applications Engineer, I like to keep my eye on the SOLIDWORKS Forum so that I can pass on advice when questions are asked. Occasionally, I’ll find a question that has been asked that is best answered with a step by step guide rather than a one line answer.

One such case is a question that was posed recently by a SOLIDWORKS forum member who asked “how to make a threaded hole using holewizard on non-planar surface (cylindrical surface)?”

There are a few replies on similar questions on the SOLIDWORKS Forum which indicates that this user is not the only user with this question. Below is the process that I have used many times for adding hole wizard holes onto cylindrical faces that hopefully you may find useful.

This example is based on a cylindrical tube that I would like to add a tapped hole to.

I find that the easiest starting point is to generate a reference plane for positioning the hole, as often the standard planes are not suitable for positioning.

Step 1: To generate the positioning plane (Insert > Reference Geometry > Plane), select the cylindrical face so that the plane is tangential to the face. Then select another piece of geometry (in this case the Top Plane) so that you can choose the angle of the new reference plane.

 

 Step 2: Once the plane is in place, select start the Hole Wizard tool (Insert > Features> Hole > Wizard), and select the type of hole that you would like. Then click on the Positions tab. At this stage, you can now select the new reference plane to generate a 2D sketch. But for this example, I have chosen the 3D Sketch button to demonstrate how to use this option. When using this option, SOLIDWORKS allows you to sketch directly onto the cylindrical face and will dynamically preview the hole location before you click to place the hole.

Step 3: Whilst adding locations for the Hole Wizard, SOLIDWORKS used standard sketch tools. Once you have clicked to place a hole, you can then switch between the sketch tools in the Command Manager Sketch tab. To allow me to add the required relations and dimensions to the 3D sketch that will locate the hole, I first added a construction line that was Coincident with the centre of the hole, and also with the circular end edge of the cylindrical face.

To define the geometry, I then added in an On Plane relation between the between both ends of the line and the plane that was created in step 1. Finally, I added a dimension to the line to specify the distance of the hole centre from the end of the cylinder.

 

One of the main reasons that I use this method for applying Hole Wizard Holes to cylindrical faces is that it gives me the best editing capability. Due to the creation of the reference plane tangential to the cylindrical face, if the diameter of the cylindrical face changes, the plane and all associated geometry will update automatically. As well as this, the angle of the reference plane can be changed to modify the angle of the threaded hole. Also, the hole position along the cylinder is controlled by a single dimension from the end of the cylinder.

Design Checks for SOLIDWORKS Electrical

SOLIDWORKS Electrical Design Check #1 - Duct Filling Ratio (%)

SOLIDWORKS Electrical Schematic is a powerful 2D software to produce electrical wiring and cabinet designs. However, with just 2D there are limits on how you can visualise and verify your design. This is where 3D modelling comes in to play. With the additional Electrical 3D, you’ll be able to see a detailed finished product before it reaches the manufacturing stage. Also, within the 3D environment, there are tools which can help to aid in your design. For example, when it comes to choosing what size of ducts to use in your design, it usually involves manual calculations or guess work and sometimes it will be at the stage where the cabinet is built before knowing what size to use. With SOLIDWORKS Electrical 3D you can calculate the Duct Filling Ratio very easily.

After routing the wires, select Calculate Cable Duct Filling Ratio under SOLIDWORKS Electrical pull-down menu. Then click on the Calculation of cable duct filling ratio in the Command complete dialog.

 

To display the duct filling ratio, right-click the on the duct component and select Properties. Within the Part Properties dialog you’ll be able to see the duct filling ratio in the list.

 

 

 

SOLIDWORKS Electrical Design Check #2 – Voltage Drop Calculation for Cable/Harness

How do we calculate the voltage drop?

A simple answer to this question is to use Ohms Law. For most cables the resistance of the cable per meter will be defined by the manufacturer and we can multiply this by the length of the cable. Then apply ohms law V_drop=IR to give us the voltage drop across the cable.

With SOLIDWORKS Electrical Schematic we can easily generate reports to display voltage drop and power loss across a length of cable or cables in a harness.

 

The information needed for the voltage drop and power lost calculation:

·         Voltage drop (V/A/km)

·         Length of cable (m)

·         Full Load current (A)

·         Applied voltage (V)

·         Inrush factor

This information will be added to the cable properties.

Important note: For SOLIDWORKS Electrical to generate a report the “Do calculation” box must be checked.

 

To generate the report go to Design rule check under Project tab. Within the Design rules manager you can add the voltage drop template that you wish to use, it would be a choice for cables or cables in harness. Once the appropriate template has been selected you will be to see the populated columns. To produce a report, select Generate Drawings and within your project documents you’ll be able to see a new report drawing is added.  

 

Resetting the SOLIDWORKS registry

Over time within SOLIDWORKS it is possible to make a wide array of customisations to your user settings and also your user interface. It can be hard to keep track of these changes if you are editing them on a daily basis like I do. Also, we all know that system updates have been known to damage registry files that SOLIDWORKS needs to be able to function correctly.

So if you would like to fully reset all of your SOLIDWORKS preferences, or if you have noticed strange behaviour or missing icons since a recent Windows update. One option to resolve your issues it to reset the registry entry for SOLIDWORKS.

Firstly, be very careful when making modifications to the registry as this may cause serious instability on your system. As such, you will need full administrative permissions on your computer to be able to edit them.

The following guide illustrates how to create a fresh copy of the SOLIDWORKS registry for the current user of the machine in a Windows environment. This registry includes the system options and customisations that a particular user has set up. Examples of the types of elements that this controls are file locations, custom toolbars and system options. By creating a fresh copy of this registry, you will revert SOLIDWORKS for the current user back to default settings as if SOLIDWORKS is a new installation.

This process will not work correctly if SOLIDWORKS is currently running, so the first step is to save all relevant work and exit SOLIDWORKS.

The registry is controlled by your operating system and in Windows the process for   accessing the registry is as follows;
 

Click on the Start button in the bottom left of the desktop and in the search dialogue type ‘regedit’

This should find the regedit.exe program and if you click it from the list, the program will open.

 

 

In the Registry Editor window that is opened, expand the folder for HKEY_CURRENT_USER to find the subfolder for Software.

 

 

 

Within the Software folder, scroll down to find the folder called ‘SolidWorks’ and expand it. This folder contains multiple folders that control different aspects of SOLIDWORKS on your machine. There are separate folders listed here for each different version of SOLIDWORKS that is installed on the machine. In the imager to the right, you may see that I have multiple versions (2012,2013, and 2014).

It is always advisable not to make permanent changes to the registry without first checking that they will not damage your system. As such, at this point you can right-click the folder that represents the version of SOLIDWORKS that you want to reset (in this case 2012), and select to Rename the folder.

 

 

 

Rename the folder to something recognisable as shown in the image to the right by adding a suffix to the name. This ensures that the folder will not move when the folders are next sorted alphabetically.

 

 

 

 

 

 

 

 

 

 

 

Now that the Registry folder for that version of SOLIDWORKS has been renamed, when the software is next started and attempts to read the registry it will be unable to locate it. This forces SOLIDWORKS to create a new registry folder with a fresh set of the default registry keys in it, essentially resetting the software options to what they were when SOLIDWORKS was first installed. When launching SOLIDWORKS for the first time after renaming this registry folder, you will be asked to agree to the end user license agreement and treated like a new user.

 

 

If you would like to check the Registry Editor again at this point, either by opening a new session (as per step 1), or by selecting View – Refresh (f5) in the menus of the Registry Editor, you will see that a new folder has been created with the same name as the original folder that you renamed.

This is an important point to make because having the new copy and the original renamed folder allows you to revert back to the previous settings should the generation of a new registry folder fail to solve any issues, or if you would like to revert back to your previous settings. The process for reverting back is very simple. Ensure SOLIDWORKS is closed, delete the ‘new’ registry folder created in the above steps, and then rename the original folder back to its original name.

When an ‘off-the-shelf’ Spring just won’t do….. Part 2

It’s always great to get feedback and requests for content and following our last blog, we got a request for an example of detailing the end of a spring with some closed coils and hooks or tabs.

Here’s an example of one way that the tools in SOLIDWORKS can be used to create a more advanced spring end including some closed loops and a small tab. The tab can be made as simple or complex as you need it to be, the process would still be the same.

 

Firstly, I started with some circular sketch geometry centred at the origin of the part to create a Helix. But this time, in the options for the Helix instead of making it a constant pitch, I chose to make a variable pitch Helix. A table is displayed in the property manager and SOLIDWORKS will generate a Helix with a smooth transition between pitch values at the specified revolution counts. It is important to allow for this in the table by specifying a number of revolutions at the same pitch and then a smaller number of revolutions for any change in pitch.

In this example I have applied revolutions 0-3 with a 3mm pitch, then in the space of one revolution (3-4) the pitch changes to 12.5mm. The pitch stays at 12.5mm for 6 revolutions (4-10), and then it reduces to 3mm between revolutions 10 and 11. Finally, there are three more revolutions at 3mm (11-14) to keep the spring symmetrical. You may also notice that you can also control the diameter of the Helix. This allows you to create tapered Helices.

Because I centred my circular sketch at the origin, my Helix is also centred at the origin. This makes it easy to put in a centre line on one of the standard sketch planes as reference geometry.

From this centreline sketch, a reference plane can be added by selecting the line and the end point to fully define the reference plane. This reference plane is to be used for creating geometry that is flat to the end of the spring rather than angled like the Helix.

Next, a sketch can be drawn onto the newly created plane to define the tab at the end of the spring. In this example, I created a centre-point arc based at the origin with no dimensions. This is because I want to relate the arc to the Helix. You will need to rotate your view slightly to be able to select the arc and Helix end points and then add in a ‘Pierce’ relationship to connect the two pieces of geometry.

 

 

 

Next, I added in the detail for my tab at the end of the spring. I have created this all in the same 2D sketch, but it is possible to create a new 3D sketch to allow for any possible tab geometry.

This process can then be repeated at the opposite end of the Helix.

Once the opposite end of the Helix has been added to, the spring is nearly ready. However, at the connection between the Helix and the flat sketch for the tab, there is a change in angle which may cause a small ‘kink’ in the end of your spring.

SOLIDWORKS has a sketch tool that will automatically neaten this up for you with very little input.

Generate a new 3D sketch and go to Tools – Spline Tools – Fit Spline. This tool will generate a single spline curve that mimics the geometry that you select to a tolerance that you specify. By selecting the sketches at the top and bottom and also the Helix curve, and making the tolerance value sufficiently small, the spline that is generated will exactly match the desired spring. Increasing the value of the tolerance will ‘round off’ any sharp edges or corners such as the connection between the Helix and the 2D sketches. In the property manager, deselect the option for ‘Closed Spline’ as this will attempt to close the loop between the 2D sketches.

 

The resulting geometry is a single spline curve that is fully defined that we can use as a sweep path for the spring. A little tip at this point is to hide all of the unrequired sketch and reference geometry by selecting it in the Feature Manager Design Tree and selecting Hide. This not only keeps your graphics window nice and tidy, it also makes for easier selection when using the spline for feature use.

 

Next, a reference plane was easily created by selecting the spline and one of the end points of the spline. This generates the ideal reference for creating a sweep profile sketch as it is perpendicular to the spline that we will use for the sweep path without having to work out any angles or measurements.

For this example I sketched a circular profile of 2.5mm diameter.

Lastly, in the Command Manager, choose Swept Boss/Base. Because all of the preparation work has been carried out and only two sketches are visible in the graphics area, it is simply a case of selecting the circle as the Sweep profile and the 3D Spline as the Sweep path to create your spring.

***

Duncan Crofts CSWE is an Elite Applications Engineer at TMS CADCentre.

 

When an ‘off-the-shelf’ Spring just won’t do….

Here’s a little tip based upon a recent request from one of our customers. They asked if there was any way that SOLIDWORKS could help them to create a square spring.

Firstly, you will need some circular sketch geometry to base a Helix curve on.

 

For this example, I created a 100mm circle on the top plane.

With the circular geometry in place a Helix can be specified easily from the Command Manager under Features – Curves – Helix and Spiral.

The Helix that you specify should have the same values as the required end result spring. In this case, 10 revolutions at a pitch of 10mm.

The next step in the process for creating the spring is to create a new 3D sketch and use the Convert Entities tool from the Sketch tab of the Command Manager to convert the Helix. This then allows you to hide your original Helix and also gain all of the benefits of using a 3D sketch.

 

The next piece of sketch geometry that you will need is a single line that is larger than your intended design of spring and sketched on the same plane as the circle used to define the Helix. The line should be Coincident with the centre of your Helix, and I have made this line intentionally unrelated in any orientation (i.e. vertical). I can then make the line Coincident with the endpoint of my converted 3D sketch.

 

The next bit of sketch geometry that you will need is the profile that you would like your spring to be. In this example I have used a square that has filleted corners, but the shapes that you can use are as varied as your imagination.

 

 

Now, let’s start construction of the spring. Firstly, use a Swept Surface using the single sketch line as the profile and the converted Helix on the 3D sketch as the path.

 

Secondly, we need an extruded surface based upon the final profile that we want the spring shape to be. This Extruded Surface needs to be the same height or larger than the original helix. You can use the Up to Vertex option to match the height of the existing geometry for this.

 

 

Now that we have the two surfaces, we can use SOLIDWORKS sketch tool ‘Intersection Curve’ to do all of the hard work for us.

Within the tool, select all of the faces or you can select the surface bodies from the feature manager. When you accept the selections, SOLIDWORKS will generate a 3D sketch exactly where the faces intersect. In this case, giving a helical incline around the square profile.

 

 

 

At this point, you can hide the surface bodies leaving only the 3D sketch of the square spring visible.

 

The last step in creating the square spring is to give it a material thickness. The most common way of doing this is to use a Swept Boss, but first we will need a profile sketch for the material thickness.

The ideal location for a profile sketch for a Swept Boss is at one end of the sweep path and in an orientation perpendicular to the angle of the start of that path. SOLIDWORKS has a function for generating a reference plane that exactly satisfies this need.

We can create a reference plane using the line at the start of our square helix as the first reference, and by selecting the end point of the same line, SOLIDWORKS will automatically position the new plane perpendicular to the line and coincident with the end point.

 

 

Now that the correct sketch plane is in place, a simple profile is added for the spring material profile.

 

The Spring can now be finalised by creating a Swept Boss Base selecting the spring profile and the profile sketch and our square spring path as the path sketch.

 

 

 

 

 The spring doesn’t have to be square though, the limit is your imagination.