Category Archives: Tech Tips

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.

Posted in Tech Tips | Tagged , , , , |

In my last tip I described how to color your skeleton or layout sketches.  That tip is great for highlighting skeleton sketches that are used to Layout a model with information essential for capturing Design Intent.

Another procedure for capturing Design Intent is to generate a sketch with Blocks to Layout an Assembly*.   Although a great technique, the Blocks are created in the same color.  The default color of your sketch Blocks are controlled by the Inactive Sketch color setting.  Additionally the Line Format toolbar could be used to add a color to the entire sketch from the feature tree, thereby coloring all the Blocks in that sketch.  However, as stated above, the Blocks are still shown in the same color, yet they represent different components in your Assembly Layout.  And unfortunately the Line Format toolbar does not allow you to ‘color’ these individual Blocks.

*To sum up this technique for my tip; a Block could represent a part or a sub-assembly in the Assembly Layout.  These Blocks can be related to one another using sketch relations.  The sketch relations between the Blocks represent mates that would be created between the modeled components in your final assembly. This layout technique using Blocks can be used for the checking of clearance and motion between components for proof of concept, before spending the time modeling the parts.  Obviously valuable as you can avoid early mistakes which saves time. See below for more information on Layout Based Assembly Design.**

For ultimate clarity it would be beneficial to color the individual Block ‘components’.

In order to color individual Blocks, select the block from the feature tree and use the command found under the drop down menu, Edit>Appearance>Sketch/Curve Color.

edit curve color.gif

When you exit the layout sketch the Inactive Sketch color will override the individual Sketch/Curve colors, thus the Sketch/Curve colors are only visible when editing the layout sketch.

color display mode.PNG

Also worth mentioning is the toggle of Color Display Mode from the Line Format toolbar as this will revert from your chosen Sketch/Curve color override back the default sketch define color status.*(This toggle is necessary to show the status of your individual sketch entities/blocks to specify if it is under defined or not.)

**For more information about the Layout modeling technique, please check out our webcast on Layout Based Assembly Design.  In that presentation you will learn about grouping sketch elements together by forming Blocks.

Posted in Tech Tips | Tagged , , , , |

With Flow Simulation 2016 users no longer have to model two separate solid bodies for use with the Two-Resistor Component feature available in the Electronics Cooling module.  To add a Two-Resistor Component model to your Flow Project, simply open the property manager and select the top surface of the one component that represents your chip.  This selected top face will represent the case node and the software will automatically populate the “Components to apply the Two-Resistor” field with the corresponding part file.  The bottom face of the component is still considered the board node and defined automatically.  The top and bottom faces representing the case face and the face touching the board still need to be parallel to one another.

For older projects that have existing Two-Resistor Components already assigned, those instances will be automatically converted to the new style feature.  You will not have to re-apply these instances.  Simply edit your Two-Resistor Component feature created in a previous version in 2016 and you will be given a message to perform the conversion.

Flow Simulation will simply add both the case and junction bodies to the “Components to apply the Two-Resistor” field and choose the case surface.

Another benefit to the change is that you no longer need to enter the dimensions of the chip when creating your custom Two-Resistor Components in the Engineering Database.  The program can automatically determine the width, length, and thickness of the structure.

 

Please note that multiple bodies can still be selected to represent the chip however their faces must be touching just as in previous versions.  This will allow you to continue using older geometry but will allow you to re-assign with a “new style” Two-Resistor Component feature if necessary.

 

Posted in Tech Tips | Tagged , , , |

When modeling in SOLIDWORKS, its very useful to have Temporary Graphics available to really see what is being added or removed from the model before the task is completed. We have been contacted regarding why Temporary Graphics will not show the correct geometry preview when Draft is enabled in a Boss/Base Extrude, or Cut Extrude.

Below you can see that the Draft Option was selected for the Boss/Base Extrude, but is not previewed.

To make the Draft visible in your Temporary Graphics you will need to adjust your System Options. Tools>Options>System Options>Performance>(check) Use shaded Preview. This will fill in your “wireframe” view of your temporary graphics and show a more accurate representation of the new intended feature.


 

After these options have been adjusted you will now see the Draft option being applied to the Boss/Base Extrude and Cut Extrude. 

Posted in Tech Tips | Tagged , , , , , |

In SOLIDWORKS Electrical Schematics there are 2 basic ways to add a new manufacture part to the ‘Manufacturer parts manager’ library. First method is to open the ’Manufacturer parts manager’ and click the ‘Add manufacturer part’. The difficulty with using this first method is you need to know the Classification, Number of Circuits, Circuit type and number of terminals per Circuit, in order to make the new manufacture part. This Tech Tip is going to go into the second method which I find easier to create new manufacture parts on the fly and add it to the library for future use.

Follow these simple steps to add a new manufacture part

1) Draw your new wire(s) of your schematic, add a symbol that represents the type of device that will represent the new manufacture part you wish to add. This typically will open the  ’Symbol properties’ window automatically, if it doesn’t, right click over the symbol and select ’Symbol properties’

2) On the ‘Symbols properties’, select the ‘Manufacturer part and circuits’ tab, click the ‘Add manually’, this will open the ‘Manufacturer part properties’

3) On the ‘Properties tab’ fill in ‘Reference’, select the Manufacturer from the pull down menu or type in if new, the class will be set already from the symbol that was used. Add additional information if you so choose.

4) On the ‘Circuits, terminals’ tab there will be one or more circuit(s) already created with the correct circuit type(s) to match the symbol that you picked.

5) If you choose to type in Terminal marks select the circuit on the top half and then type in the Marks below.

 When you click OK, you’ll be prompted to add it to the part to the catalog. If you click yes then the manufacture part that you just created will be available for other schematic users connecting to the same company Electrical server and future schematic projects.

 

Aside from manually adding new manufacture parts as mentioned here, you can first start out by checking a download of manufacture parts libraries from the ‘SOLIDWORKS Electrical Portal’ to see if it contains the part you need.

http://www.solidworks.com/sw/products/electrical-design/solidworks-electrical-contentportal.htm

If this is your first time to the site register for a new account.

 

Posted in Tech Tips | Tagged |