With the new version of SOLIDWORKS just around the corner or when your company buys more licenses, it’s important to know that an extra step is required to start using the new, or additional floating/network licenses for SOLIDWORKS, PDM, Composer, and Electrical. This tech tip is a guide to walk you through installing the SolidNetWork License Manager (SNL) required for these licenses.

*If you just purchased additional license for an existing Network serial number skip to Step 3).

Step 1) Locate which computer system you want to install the SNL, or locate which system is already running the SNL that you are needing to update.
When you’re company already has network licensing in place, the best way of determining which system is your SNL server is to open the SolidNetWork License Manager on a client system.
Windows Start menu > all programs > SolidWorks 2016 > SolidWorks Tools > SolidNetWork License Manager >  Server List tab
For system requirements as to what type of system you can use - http://www.solidworks.com/sw/support/SystemRequirements.html - SOLIDWORKS Network License Server section

Step 2) *If you are not changing major versions or installing new please skip this step (i.e. 2015 to 2016).

To install or update the SNL either download the SOLIDWORKS Install Manager that matches the major version of SOLIDWORKS that you’ll be using, or insert the SOLIDWORKS DVD into the selected server (Service pack can be different from the server and the client, I like to have the latest service pack when i’m installing or updating the SNL).

If you have a download of the SOLIDWORKS install files just run the ‘setup.exe’ to Start the SOLIDWORKS Install Manager. Select ‘Server Products’ then either check ‘Install SolidNetWork License Manager’ or if you are upgrading check ‘Upgrade SolidNetWork License Manager’
(If you are upgrading you may want to un-check the other products that your company may not be ready to upgrade just yet). Walk through the steps to install the SNL, it will ask for your network serial number(s) and finish. (Side note: SOLIDWORKS network serial numbers the 3rd digit is a 1. (i.e. The first 4 digits are commonly 0010…, or 9010…)

Step 3) Once the install manager has is either upgraded, or installed, the next step is to activate the licenses. When the SNL install is new, activation pulls down the licenses based on the serial number(s) that where entered during the install process. When the SNL is upgraded, or new licenses are purchased it will add the additional new licenses when reactivated. To open the SolidNetWork License manager on the server after the install go to:
Windows start menu > All Programs > SolidNetWork License Manager or SOLIDWORKS Tools, then open the SolidNetWork License Manager Server 2016.

During the first launch after the install you will either be prompted to activate.

If you are adding licenses, the SNL manager will open without a prompt, we will then want to click on the ‘Modify’ button on the ‘Server Administration’ tab to reactivate.

Then select the middle option ‘Activate/Reactivate your product license(s)’

Step 4) When reactivating you will be prompted if you are using a Firewall, this is a good option to have checked whether you’re using a firewall or not. It locks down the incoming/outgoing ports.

Step 4) Click the Next button to select the serial numbers that you want to activate. Most companies only have 1, but you can still click the select all. Enter in your email address to be logged with who activated the license. If the computer is connected to the internet you can activate ‘Automatically over the Internet…’, otherwise select ‘Manually via e-mail’.

Step 5) *For Manual activations only* – select 1 serial number at a time, click next, then you will be presented with a screen to save a request .txt file that will need copy or moved onto a system that has email access. The request file gets sent to: activations@solidworks.com

IMPORTANT: Leave this Manual Activation screen open so that you can read in the response .txt when you receive the automatic response a few minutes later. (The computer can be locked but you must leave the Manual Activation screen open because the request and response files are time stamped to each other.)

With a Manual activation most likely the first time you activate a SNL server you will be prompted to do a second request .txt to get a second response .txt

Step 6) Once the SNL is activated, the final step is to verify that you have the correct quantity of licenses that you purchased. Remember for every seat of SOLIDWORKS Professional or SOLIDWORKS Premium you also see a seat of SOLIDWORKS Standard. SOLIDWORKS Standard is the main program, where  SOLIDWORKS Professional and SOLIDWORKS Premium are the upper level add-ins.

Posted in Tech Tips |

Part of the fun in teaching SOLIDWORKS is showing some of the time-saving shortcuts available to make students more efficient. This helps make the software easier to use and gives users more time to focus on what’s really important: their designs. It is hard to remember all the shortcuts and there really isn’t a complete, master list out there. This tech tip is a good start on documenting some of the available shortcuts, focusing on four keys on your keyboard. They are Shift, Ctrl, Alt, and Tab keys.

I will cover as many of these commands as I can in this article for the four modes of SOLIDWORKS; Sketch, Part, Assembly and Drawings. The intention of this article is to try go over the not so obvious commands that you might not know, especially helpful for new users. I hope you enjoy this list and that it helps you become more productive while you are designing in SOLIDWORKS.


  • Dimension to the tangent of an arc or circle (min/max condition) – Hold down Shift while using Smart Dimension
  • Move a series of entities – Hold down Shift and drag the selected entities to another location
  • Zoom larger or smaller– Hold down Shift and the middle mouse button while moving the mouse up and down. This will zoom about the screen center and is smoother and more responsive than spinning the scroll wheel
  • Copy a series of entities – Hold down Ctrl and drag the selected entities to another location
  • Turn off automatic relations and/or grid snap – Hold down Ctrl while drawing entities
  • Move multiple spline points at once – Ctrl select points and then drag any of the points*
  • Change spline controls symmetrically – Hold down Alt while dragging a spline control arrow
  • Change XYZ direction in a 3D sketch – Click Tab while drawing entities in a 3D sketch

Part Documents

  • Move Features – Hold down Shift and drag a feature to another location (Disable Instant3D)
  • Select transparent items – Hold down Shift when attempting to choose a transparent face on a part, or vise-versa when System Options, Display/Selection “Select through transparent items” is turned off
  • Copy Features – Hold down Ctrl and drag a feature to another location (Disable Instant3D)
  • Switch to another open document – Hold down Ctrl, then click Tab between each one
  • Create a new offset, parallel plane – Hold down Ctrl and drag an existing plane
  • Change advanced settings of an appearance or scene – Hold down Alt when dragging an appearance or scene from the appearance tab in the task pane
  • Rotate in 90 degree increments – Hold down Shift plus your arrow keys
  • Rotate clockwise/counterclockwise in 15 degree increments – Hold down Alt plus your arrow keys
  • Pan the Model – Hold down Ctrl and drag your middle mouse button or use your arrow keys
  • Reference Triad – Hold down Shift  and click selected axis to rotate view 90 degrees,
  • Reference Triad – Hold  Alt and click selected axis to rotate view 15 degrees
  • Magnifying Glass – Use Ctrl and middle mouse to pan the magnifying glass
  • Magnifying Glass – Use  Alt  and middle mouse to section in the magnifying glass
  • Hide Solid or Surface Bodies – Select Tab with mouse hovered over the body*
  • Show Solid or Surface Bodies – Select Shift + Tab with mouse hovered over the body*
  • Flip the direction of a formed feature (Sheet metal) – Click Tab while dragging the feature to a face

Assembly Documents

  • Select multiple components – Hold down the Shift key when window selecting components with other components already selected
  • Smart Mate – Hold down Alt, click and drag an edge or face to another component to mate
  • Smart Mate + Copy Component at same time – Hold down Ctrl + Alt, click and drag an edge or face to another component
  • Copy a Component – Hold down Ctrl and drag a component to another location
  • Hide a Component – Select Tab with mouse hovered over the component*
  • Show a Component – Select Shift + Tab with mouse hovered over the component*
  • Invert selection – Hold down the Ctrl key when window selecting components.  Components that are already selected will become deselected
  • Select a transparent face – Hold down Shift when attempting to pick a transparent face, or vise-versa when System Options, Display/Selection “Select through transparent items” is turned off
  • Change direction of the move function when using Move with Triad – Hold down Alt and move the triad to an edge to change the direction
  • Change from reorganize to re-order while moving parts in the Feature Manager Design Tree – Hold down Alt while re-ordering parts in the feature manager so you don’t accidentally add a part to a subassembly
  • Copy a part from one assembly to another – Hold down Ctrl while dragging the part to other tiled window
  • Change direction of Routing components – Hold down Shift plus your left or right arrow keys to change the orientation of a routing component upon insertion
  • Mouse gestures – Right click drag over a component rotates it, so hold down Alt if you meant to use mouse gestures
  • Create parts instead of configurations when using Toolbox – Hold down Ctrl when dragging a part into your assembly
  • Camera Views – Use Ctrl, Shift, and Alt keys plus your middle mouse button to manipulate camera views
  • Walkthrough – Use Ctrl, Shift, and Alt keys to change the orientation of your camera while using the walkthrough function
  • Motion Manager – Use Ctrl and Alt keys to copy and move multiple keys in the motion manager

Drawing Documents

  • Move child views with the parent – Hold down Shift while moving the parent view
  • Move model items between views (Dimensions) – Hold down Shift and drag an item from one view to another
  • Break the alignment of Geometric Tolerance Block (Feature Control Frame) from a Dimension – Hold down Shift and drag the frame away from the attached dimension*
  • Select cells in BOM – Use the Shift or Ctrl keys and pick the cells you want to edit
  • Break alignment of views – Hold down Ctrl during the creation of a projected view
  • Copy a sheet to another drawing document – Hold down Ctrl and drag the sheet while windows are tiled
  • Copy model items between views – Hold down Ctrl and drag an item from one view to another
  • Add additional leaders to a note – Hold down the Ctrl key while dragging the arrow
  • Move annotations without snapping to the grid or other annotations – Hold down Alt key while creating or moving
  • Move tables (BOM, revision) – Hold down Alt and you can drag the table by picking any place on the table
  • Move an annotation independently in a group – Hold down Alt and drag annotation
  • Move views – Hold down Alt and you can drag the view by picking any place within the border

One final general note, as you can see in the list above, is that Ctrl selecting and dragging an item usually makes a copy in SOLIDWORKS. This is true in sketch, part, assembly or drawing mode.

*denotes new addition to previous tech tip posted 3/15/2011

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With the release of SOLIDWORKS 2016, they incorporated a new function with Sketching called Instant2D. It is located on your Sketch command Tab. FIG1

While working with Instant2D active, this feature functions like Instant 3D but at the sketch level. You will notice that there are Blue Grab dots at the end of your Dimensions (FIG2). With these Blue Dots you are allowed to grab and drag the Dimension to the desired size. This is a great function if you are working on a conceptual design and looks are more important than the exact measurements.  Note: These Drag dots are only applied to driving Dimensions.

You will however notice some differences on selecting dimensions while Instant2D is active. The most common one that a user will notice is the Modify box will not come up. Instead it is a simple cell that has the Dimension value listed (FIG3).

You are however able to still insert the exact desired dimension using this. You just don’t have as many functions as you would with the Modify Box (FIG4).

The second noticeable change is that if you select a dimension text and then press Delete. SOLIDWORKS will not delete the dimension; instead it will bring up the simplified cell to change the dimension. If you do not notice this you will accidently delete the value of that dimension, then SOLIDWORKS will send a warning that you can’t have a dimension with no value (FIG5)

To move beyond this delete issue, you will need to select the leader line then press delete.

The Instant2D function may not be for everyone, but it is a great tool that SOLIDWORKS has added to their Sketch functions. Many product and conceptual designers will find this very useful.


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It is a scary thought, knowing that adjusting your lights and scenes in SOLIDWORKS could cause the display of your Simulation result plots to change.  This is indeed true, however it is not as scary as it first sounds.

The behavior is actually that the brightness of the Simulation Color Plots are dependent upon the light definitions and lighting scenes in SOLIDWORKS.  This occurs since Simulation resides within the SOLIDWORKS ecosystem which is great for changing models on-the-fly and re-running a study, however adopting the lighting of the CAD model is one of the drawbacks.  The behavior can be seen in the below screen capture and is exaggerated by turning off some directional lights.  The good news that using the most common lighting scenes this behavior is not very noticeable and most of us won’t run into anything these exaggerated unless lights are changed manually.

Turning off two directional lights caused a noticeable difference especially between the yellow and green colors in the plot and can cause confusion and misinterpretation of the results going from the color bar to the colors mapped on the model.

If you are running into this behavior or want to avoid this behavior all-together, simply turn off all directional lights, edit the ambient light and slide the slider all the way to full capacity.  This will give you a true representation of the colors as seen on the color bar for the best comparison possible.


This is a behavior that a significant amount of users have reported in our community, in fact there is a current enhancement request out for this specific behavior:  SPR:  887500- “Ability to define default scene for viewing simulation results (no directional light, all ambient).”  We hope to see this updated in a future service pack or major update.

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I recently ran in to a need to create a few structural brackets for framing up a new deck.  I found that one manufacturer didn’t have 3D CAD models to download but they did have .dwg files that I could download and create a 3D model from. So I brushed off some cobwebs on how to use the built in 2D to 3D tools built in all version of SOLIDWORKS and thought I’d share my relearning with everyone.

Step 01 – Download the dxf or dwg that you need. For this example I’m downloading a dwg of a Joist Hanger from https://www.strongtie.com/ . Their download site is https://www2.strongtie.com/drawings/   at the time of this posting. If you look at the screen capture from their website they’ll give you a few options and I found that the top option includes the front, left, right and top views all in a single dwg.

Step 02 – Open the dwg in to SOLIDWORKS. Here are the settings that I use:

Setting 01 – 2D Sketch

 Setting 02 – Optional to have constraints added

Setting 03 – This is a good option to have on because your model creation will be easier if you have clean sketches.

Once you hit finish SOLIDWORKS creates a single sketch of the 3 different views. This sketch may need some cleanup. Lines that don’t connect to arcs, etc… A single sketch is created if all three views are only on 1 layer in the original dxf/dwg. When SOLIDWORKS finishes importing the model you will most likely see the 2D to 3D toolbar turned on on the left side of SOLIDWORKS. This 2D to 3D toolbar can also manually turned on.

Step 03 – Now we need to position the sketches in to the correct orientation by using the different ‘Add to…’ buttons on the 2D to 3D toolbar. We first start with the ‘Add to Front sketch’ button. While still editing the sketch that was imported, select all of the sketch entities that make up the front view and then click the Add to front sketch’ button.

Step 04 – Then we’ll go though and select the additional sketch entities that make up each of the different views and then click the corresponding ‘add to…sketch’ button. Top, Right, Left, ….  as many as there are that pertain.

You’ll see that after the ’add to…sketch’ button is clicked, the sketch entities will then rotate to their new orientation. You can exit the original sketch and you should see something like the image below.

Step 05 – In this step we’ll use the ‘Align Sketch’ button on the 2D to 3D toolbar to align the sketches with the origin or the other sketches. 

The way this button works is, you select 1 point on 1 of sketches and click the button and it will shift this sketch to align the selected point to be perpendicular to the origin. Or if you select 1 point of one sketch and 1 point of another sketch it will align theses point. It may be necessary to edit some of the sketches and add sketch points to assist with alignment. A trick that I’ll use is ctrl select two lines then click the sketch point button, this creates a virtual sharp sketch point, while editing the sketch.

With all of the sketches brought in from the dxf/dwg files and aligned, the last step is to create your 3D model. In the case this being a sheet metal part here are my basic steps for this part.

Step A – Start a new sketch on the front plane and convert entities of just the inside edges. Then use the ‘Base Flange/tab’ to extrude up to vertex.

Step B – Use the side sketches to create cut extrudes sketch/features that remove the extra material.

Step C – Complete the part using edge flanges, cut extrudes, tabs and forming tools.

Happy converting.

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