Thursday, 19 June 2014

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.
 

Thursday, 5 June 2014

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.
 
 
 
 

Thursday, 1 May 2014

Seamless collaboration between Electrical and Mechanical design teams



Over a year ago SOLIDWORKS added a new Electrical package to its family of products. SOLIDWORKS Electrical simplifies electrical schematic creation with an intuitive interface just like SOLIDWORKS 3D CAD.

SOLIDWORKS Electrical has helped companies to improve time to market and reduce development costs by eliminating wasteful processes among electrical and mechanical design teams. It provides collaborative environment, in which all electrical and mechanical designers not only share symbol and component libraries, but with the ability to work simultaneously on the same projects.  The SOLIDWORKS Electrical project server keeps everyone up-to-date with the latest changes in real-time.


Bidirectional integration in real time with SolidWorks 3D

 

The advanced tools in SOLIDWORKS Electrical 3D makes it easy to create auto-routing of wires, cables and harnesses. The information of wire length can be generated and then be finalised to the Schematic reports. 

It’s very easy to route the wires in Electrical 3D, simply select ‘Route Wires’ command and ‘hey presto!’ done. By using the’ SolidWorks Route’ option you can create a more realistic effect. It is also possible to segregate wires so that specific wire styles will not route along selected sketch path.
 
 
In 2014, SOLIDWORKS Electrical Schematic can be installed using SOLIDWORKS Installation Manager, making it a one simple process to install both the Mechanical and Electrical software, keeping the I.T guy very happy.


Comprehensive library is shared across Electrical and Mechanical users. SOLIDWORKS Electrical offer over 500,000 manufacturer parts in the library database but if there are parts which is not available you can still download the data from various resources such as tracepartsonline.net, 3D Content Central, etc.
 
www.tracepartsonline.net
 
www.tracepartsonline.net

 

Wednesday, 5 March 2014

SolidWorks Composer – Intelligent Views

Today engineers and designers are looking for more advanced ways to communicate their technical processes and procedures. With SolidWorks Composer you can create not only clear and accurate technical documentations but also contents where the user can interact.
 
Custom views, sometimes called intelligent views capture only the actors and properties you specify.
We can use intelligent view to create different configurations such as a colour selector, language translator, etc.
 
 
Language Translator
 
Not everyone speaks the same language, with Composer intelligent views we could create interactive buttons where users could select their preferred language.
 
I’m going to use a toy car as an example. Create a view layout with the annotation labels (in English) and a list of languages you wish to include.
 
 
 Turn on the View Workshop.
 
 
 
Select all the labels. (Tip: the quickest way is to use the Select tools and deselect Select Geometry filter this way you could just drag a window across the screen without selecting the model). 
 
Once all the labels are selected create a custom view and name it English. Then replace all label text to another language for example Japanese (maybe use Google translate to help) and create a new custom view.

Each View has a preview thumbnail image. Thumbnails for custom views have a diagonal line and shading.

 
 
Select the 2D text box marked English and go to the Link property to select an event URL. In this case, selecting the custom view we’ve just created i.e view://English. Repeat the procedure for the rest the languages.
 
 
 
Once complete, switch off the design mode and test the result by double clicking the different language text boxes.
 
 

Tuesday, 4 February 2014

Upgrade your SolidWorks License Today!!

Recently, TMS CADCentre has received many support calls for assistance with updating SolidWorks to include recent license modifications such as extra seats on a network, new add-ins like SolidWorks Simulation, or upgrades from SolidWorks Standard to SolidWorks Premium.
There are slightly different processes for each, and here’s a quick run-down of the main processes to follow.
 

Adding Upgrades to your Standalone seat of SolidWorks


If you have purchased an Add-in for your current SolidWorks License such as SolidWorks Simulation Professional or Premium, SolidWorksElectrical, SolidWorks Plastics, or SolidWorks Flow Simulation, you may be able to activate it through the SolidWorks user interface by selecting Help – Activate Licenses. You may need to reactivate SolidWorks first to recognise that it can now activate your Add-in. Highlight the product that you want to activate and select ‘Next’.



If you have created a custom installation of SolidWorks when it was previously installed and selected not to install the components for your Add-in, or if you have a new serial number for an upgraded or separate product, you will need to modify your installation to add the new serial number.
If you have a separate serial number for an Add-in you don’t need to transfer any licenses. But if you have a new serial number for SolidWorks, you will need to transfer the current license before adding the new one. This can be done within the SolidWorks user interface again by selection Help – Transfer Licenses. Select the components you would like to transfer and click ‘Next’.


Once you have transferred the license, you can modify the installation of SolidWorks to change/add the new serial number. Go to Control Panel - Programs – Uninstall a Program, or Control Panel – Programs and Features (depending on your Control Panel settings). Once the list of programs on your computer has populated, scroll down to find your SolidWorks installation, Right-Click it and select ‘Change’.




This will open up the SolidWorks Installation Manager for the version of SolidWorks that you selected.  On the welcome page the first option is to ‘Modify the individual installation (on this computer)’. Ensure that this option is selected and click ‘Next’. You will then be taken to the page to review and modify your serial numbers. If you have a new serial number for SolidWorks or a separate number for an Add-in, please enter them on this page.

 

Once you have entered in your new/replacement serial numbers click ‘Next’ and you will be taken to the Product Selection page. Please take the time to ensure that all of the products that you would like to have available are checked in the list shown (including any new add-in functions that you may have entered the serial number for). Clicking ‘Next’ will then take you to a summary page to allow you to review any modifications before finally clicking ‘Modify Now’.

 

Once the modification process is complete, launch SolidWorks. If you have inserted a new SolidWorks serial number, you will be asked to activate your product before continuing. If you have added a serial number for an Add-in such as SolidWorks Simulation, when you turn on the Add-in in SolidWorks, you will be asked to accept its terms and conditions and then to activate it before use.

**To turn on your Add-ins in SolidWorks, go to Tools – Add-ins.
 

To add allocations to a Network License

The number of SolidWorks seats on a network license is controlled by how many allocations there were when the license was activated on the server machine. If this number has changed, or if there are additional products to add, the license server needs to contact SolidWorks to access the new allocations.
If you are currently using the latest version of the SolidNetwork License (SNL) Manager software on your server, ensure that no licenses are currently being borrowed before making any changes and stop the license manager service. This can be done on the welcome page of the SNL Manager user interface.
Once the service is stopped, also on the welcome page is a button to ‘Modify’ the license. Click this button and the options to ‘Transfer’ and ‘Activate/Reactivate’ will be shown. As long as you are using the newest major release you can simply reactivate the software to pick up extra allocations.
If you are using a previous release of SNL Manager, you will need to install the latest version to be able to activate.
 
**Be sure to check the SolidWorks system requirements before proceeding at http://www.solidworks.com/sw/support/hardware.html .
 
Only one version of SNL Manager can be installed on a server, so you will need to transfer the license as detailed above. Then uninstall the SNL Manager program using Windows Control Panel. Lastly, either using a file set, or the media supplied by TMS, install the latest version of the SNL Manager onto the server. It is best practise to reboot the server at this point to fully complete the installation of the software, so please arrange the installation at a suitable time to be able to do this without affecting your network users.
If you have received a new serial number from TMS,  you will need to modify your SNL Manager to enter the new serial number. To do this, firstly stop the service as detailed above and then go to the Windows Control Panel and modify the installation of the SNL Manager software. This will open the SolidWorks installation manager. On the welcome screen select to ‘Modify’ and click ‘Next’. The following page will allow you to check and change/add any serial numbers that you have for the SolidWorks product range. Once you have the correct serial numbers, click on ‘Modify now’.
 
For a list of the functions and upgrades available for your SolidWorks installation, please see the image below. Or for a more comprehensive solution for your needs please call us and have a chat.