If you took any of our SolidWorks classes or perhaps saw a YouTube video, you may have noticed a discrepancy between the dimensions seen on other users’ drawings and your own. For instance, many students have noted that dimensions in drawings come in gray in some cases, and black or blue in others. This can be particularly frustrating if you have been able to bring in both colors separately without knowing. This blog will show you how to control the color of dimensions in a SolidWorks drawing.
|There are two basic ways to import dimensions in a drawing:
Smart Dimension or Model Items.
If you use Model Items, you can bring in dimensions Marked for Drawing and Not Marked for Drawing as well as other locating dimensions and annotations. Almost always, these dimensions will come in black. However, some features may not be fully dimensioned.
If that is the case, you will need to use your smart dimension tool to place what some call Reference Dimensions. These reference dimensions are also known as Non-Imported (Driven) dimensions. Almost certainly, these dimensions will be a confusing gray color.
One other significant reason that dimensions are gray is due to the layer properties. If you place dimensions on a separate layer so you can easily hide them, you may also affect the color. Look for the small color box on the layer dialog box. Is this color set to something other than black?
If so, then you should expect all dimensions and lines assigned to that layer to follow that color scheme.
The last significant reason for dimensions being gray is if someone has simply changed the color of the individual dimension through the Line Color command on the Line Format Toolbar.
Now that we have identified what causes dimensions to be gray, let’s control the colors of these dimensions.
For starters, if you used Smart Dimension to bring in Reference / Non-Imported dimensions, go to System Options> Colors> Non-Imported (Driven) located here.
Choose the Edit button and change the color to anything you would like. In this case, I changed them to a distinct red color.
If your layer has been set to gray, launch the Layers Properties dialog box from the Layers toolbar. Choose the colored square and pick another color. In this case, I chose blue.
|To change any particular dimension, select the dimension and then select Line Color and choose an appropriate color. In this case, I chose green.
I hope this has helped you determine and control the color of your dimensions in a SolidWorks drawing!
Post by Gabe Enright
Day after day our support team reports the same thing over and over. Many SolidWorks users are working in one of the most inefficient ways possible. What is that way? Working directly from a shared network drive. I am not an IT professional and will keep this discussion high level, but we will talk about the reasons why opening SolidWorks files from a network drive is bad.
Let's start with why many do work from shared locations.
- It's a convenient way to allow users to access the data they need to. Once a project is complete we need to put it somewhere and if someone else needs to access it they need to know where to find it.
- It's easy to back up. No company is going to allow its valuable Intellectual Property to exist without being regularly backed up.
Now let us discuss why this is a bad strategy for SolidWorks users.
- Its slow
No matter the speed of your network, loading something from your local hard drive is always going to be much faster. With the increasing use of SSD's that gap is widening even further. Remember opening a SolidWorks assembly may also require the loading of many other referenced components at the same time.
- It can be unstable
Remember, if you are opening SolidWorks files from a network drive there are at least two pieces of hardware involved, your computer and the server. There may also be other devices between them like switches. Any bottlenecks or failures while opening can lead to you having to start the process over. If something happens while you are saving you may end up with a corrupt component. At that point we have to get SolidWorks Technical Support involved and pray they can recover your component. If they can't, you are requesting a backup copy and redoing your work.
Here's a quick analogy. Imagine you are packing the family minivan for a weeklong road trip. A pretty inefficient way to do it would be to pick up everything you are bringing, carry it out to the car and load it without putting anything down. A sane person would bring everything out to the car, put it down then load it.
||Customers will often call frustrated that an assembly takes a long and often variable time to load. They are growing weary of waiting for the “Busy” icon to clear so they can actually do some work.
If your blood pressure is rising just seeing this, then you know what I’m talking about. We have a simple test that we ask customers to try which is to copy the data set to their local drive. This is often most easily accomplished with a Pack & Go. 9 times out of 10 they will report the assembly loads dramatically faster. Even when accounting for the time to copy the files to the local drive it is still much faster to get that assembly open this way.
So at this point we've convinced the customer that it is faster to work from their local drive instead of the network. They are still going to tell us this method is not practical, and they are correct! They now have lost the protection of having routine backups. When they are done they still have to put the components back on the network. If I copy a fifty piece assembly from the network to my local drive and change 10 parts I have to put the ten changed components back when I'm done. Perhaps they were in different folders on the network. I have to determine which components changed, and put them back. Then I should delete the files from my local drive.
That is the most basic scenario but let me throw in a couple other wrinkles. What if you want to keep the old version of the file for history? How can you be sure you loaded all the changed files back to the network before deleting them from your local drive?
The answer is you can overcome these challenges with enough time and a thorough understanding of SolidWorks referencing. Frankly, I'm guessing nobody got into engineering and design dreaming of spending hours moving files around.
There has to be a better way, and there is. The answer is Product Data Management or PDM. PDM makes all these challenges go away by: automatically moving files to your local drive to be edited, putting the changed ones back when you are done, and making sure that only one person changes a file at a time. If you are getting the idea you need PDM you might as well start with the Best PDM system for SolidWorks files, SolidWorks Enterprise PDM.
||I will be hosting a webinar introducing SolidWorks EPDM on Tuesday April 15th. Register today and join us on Tax day to see all the deductions you can take from your design and documentation schedules. Use this link to Register, or view an archive of the session if it has already passed.
Post by Jon Sorocki
Instead of recreating the same feature all the time, why not insert features into Solidworks Design Library? That way you can drag the feature out whenever you need it. This is one of the perks of using SolidWorks and should be utilized by just about everyone. In today’s post I will show you how to insert features into Solidworks Design Library.
First, let’s start with where to find the design library. By default, one is installed in C:\Program Data\SolidWorks\SolidWorks 20xx\design library where xx represents version/year of SolidWorks. The default library comes with some features and parts already. You can add other library locations by going to Tools> Options> File Locations> Show folders for: Design Library. Locating the library while in SolidWorks is simple. Look to the right hand side of your screen for a stack of books, usually located under the house icon in the Task Pane.
Now, let us create a common feature that we will store in the library. For this example I will use a logo, since having a logo to engrave or deboss is very common with customers. Create a new part and sketch out a dummy body. I like to use a 2”x4” rectangular prisms with 1” depth.
Sketch the logo on this top face. Use a Cut-Extrude feature to deboss down however much you want; I usually keep it minimal and around .02”. If you dimension any part of the logo to the edges you will be required to reference these edges every time you drop the logo in from the library. If you want to keep certain spacing feel free to use dimensions, otherwise sketch the logo free form without any dimensions or relations to existing geometry including the origin.
View your feature manager tree. You should see a Boss Extrude and a Cut Extrude. We are only interested in saving the logo out, so select the Cut Extrude from the tree. Press File> Save As. Choose file type as Library Feature Part (.sldlfp). Save to any folder in your design library or save to the root. It is absolutely necessary that you select the feature and verify that it is highlighted before pressing Save As. You must also make sure to save as Library Feature Part!
Once it has been saved, you should see a stack of books next to the part name at the top of the tree.
You should also see a small green “L” appear above the Cut Extrude icon. If this does not happen, try the Save As again. Check the design library in the task pane. You should see a thumbnail representing the logo.sldlfp you just created.
You should be ready to use this logo from your design library at any time. Simply find the part you want to place the logo on and drag-drop the logo thumbnail from the design library onto the flat face you want to engrave or deboss. If you created dimensions to edges, you will be required to select those edges again. If you left it undefined and free-form you are free to place your logo anywhere you want.
Can you run SolidWorks on a virtual machine? Virtual machines aren't supported by SolidWorks - for anything. As they say:
"Virtual environments force SolidWorks, eDrawings, and DraftSight to run in Software OpenGL mode resulting in significant graphics performance degradation."
Disclaimer to SolidWorks Users - check!
I can't speak for SolidWorks, but I wouldn't support SolidWorks on a virtual machine officially because there's too much to reasonably test. But, CADD Edge has installations of VMWare products around and we can support you from that perspective. However, if we find an issue we can't resolve, there's no "backup" from SolidWorks. So understanding the lack of official support, I was surprised to see this:
Look closely; that screenshot is a Mac. As regular readers of this blog know, I run on a Mac, so I use SolidWorks on a virtual machine (vm's) all day, every day. I don't have any performance issues, but that's a test sample of one. Recently though, we've been discussing expanding our use of VMWare at CADD Edge. After looking into the possibility, it seems that the biggest hurdle is graphics. VMWare appears to be aware of this objection to its use based on this mention of graphics-based applications:
So I dug into this with help from VMWare technical support and nVidia. As you may know, we are partnered with nVidia on the GRID computing product.
||NVIDIA GRID VCA is a turnkey network device that enables up to eight users to seamlessly run SolidWorks from a Mac, Windows, or Linux PC.
I only investigated Workstation 10. My goal is to understand how graphics work in general with SolidWorks and then translate that understanding to virtual environments.
The basic pieces used in the generation of graphics are the CPU, the GPU, and the operating system. This last item needs some clarification.
We know (or should know) there are graphics drivers and there's this thing called OpenGL. Understanding how they fit into the generation of 3D graphics will help us understand how using a virtual machine (vm) will affect the graphics.
The CPU and GPU need an operating system - say Windows 8.1. Windows 8.1 contains software to interface with different types of devices. In our case, the software interface talks to a graphics driver and not the graphics card directly. In turn those drivers talk to the hardware - in this case the GPU. For 2D and 3D rendering, that interface software is OpenGL.
OpenGL is an API used to interact with the driver and GPU to render 2D and 3D graphics. In SolidWorks, the OpenGL API is used to to accelerate the 3D rendering, also known as hardware accelerated rendering.
That's the basics. Now we move on to a vm. In the case of Workstation 10, 3D graphics acceleration is an included feature. The vm has access to the GPU. There's a switch to turn on 3D acceleration.
However, while the vm does use OpenGL2.1, the vm doesn't have access to the graphics card driver, the vm uses its own driver. As many SolidWorks users know, having the correct, SolidWorks approved driver is important. So, graphics in SolidWorks may work fine for you on a vm, but there's every reason to be concerned that it won't. I understand that VMWare is working to improve the graphics and if I hear about it, I'll let you know.
Being a geek at heart, I always love pointing out to my friends and family a product that is designed utilizing SolidWorks. When the creator is a CADD Edge customer, I get even more excited, if that is even possible! That’s why Solidworks World 2014 was so fantastic.
Sitting in the massive convention center during SolidWorks World 2014 listening to presenters speak about cutting edge, life impacting innovations can be really moving. And it’s really something special when I hear, “That’s a CADD Edge customer!” Although I should be used to it by now, it’s still exciting to discover that year after year many of our customers end up on the big stage as presentors of the general sessions. This year was no exception.
One of the most inspiring was Hugh Herr from BiOM. After discussing and showing a video about the innovative design built into his company’s bionics legs, he rolled up his pant leg. There for all to see were two of his prosthetics, which he put to use running across the stage. Seeing a double amputee walk and run naturally is truly incredible. Add on top of that the knowledge that BiOM leverages both SolidWorks and Altium to bring this life-changing technology to fruition is frosting on the cake. Then knowing that CADD Edge is their reseller, is the frosting on the frosting. After all, who doesn’t like double frosting!
Another presentation of interest was by Superpedestrian. Superpedestrian's Copenhagen Wheel captures energy as you bike when braking or going down hill which is stored in a battery helping you bike faster, further and easier. Now that sounds like my kind of bicycling.
Then there was MarkForged displaying their desktop 3D printer that prints carbon fiber parts. 3D printing can be mind blowing and MarkForged is definitely on the cutting edge creating printers that deliver high tolerance parts for production use. I just had to smile upon hearing one of our sales people say that MarkForged is also a CADD Edge customer.
Onto the timely 2014 winter Olympics. Did you know that the US bobsled is designed with SolidWorks? Yes, another CADD Edge customer… BO-DYN. As if we needed another reason to cheer on the US bobsled team to bring home the Olympic gold!
And CADD Edge’s impact didn’t end at the main stage. When walking around the partner pavilion we were able to see even more of our customers and their products – Hologic, Quirky, Makerbot, etc.
I am already looking forward to SolidWorks World 2015 to see what CADD Edge customers will be presenting their products to the entire worldwide SolidWorks user community!
Connect with the CADD Edge team and let us help you take your business to the next level with innovative software solutions and expertise you can count on.
Post By Wayne White
Teaser time…I will be going back through the AR Drone, and focusing on Plastics…using it to gain insight on weld lines, sink marks, fill and pack times, and now in 2014 SP1: warpage and cooling analysis.
One of the great things about my job is there’s always something new coming out. Dassault is a great company and all great companies will introduce new technology to keep up with consumer’s needs.
This new tool, Plastics Advanced, does some pretty cool stuff. The entire breakdown between Plastics Pro, Premium, and Advanced is below.
SolidWorks Plastics Professional
The most cost-effective time to optimize plastic parts for manufacturability is during the initial stages of product design. Skipping this step often leads to an inefficient mold design with an extremely narrow “good parts” processing window, resulting in high reject rates and time-to-market delays.
- CAD Integrated: Fully embedded in the SolidWorks 3D design environment so you can analyze and modify designs for manufacturability at the same time you optimize for form, fit, and function
- Easy to Learn and Use: Takes only minutes to learn and does not require extensive analysis or plastics expertise
- Facilitates Design Team Communication: Web-based HTML reports make it fast and easy to communicate simulation results and design advice to all members of the design-to-manufacturing team
SolidWorks Plastics Premium
SolidWorks Plastics Premium gives designers or builders of injection molds an accurate, easy-to-use way to optimize them. Quickly create and analyze single, multi-cavity, and family mold layouts.
- Avoid costly mold rework: ensure molds will work right the first time to avoid time-consuming, costly, and unnecessary rework
- Optimize feed system design: analyze sprues, runners, and gates to balance runner systems; optimize gate type, size, and location; determine the best runner layout, size, and cross-sectional shape
- Estimate cycle time, clamp tonnage, and shot size: quote tooling projects quickly and accurately; size the injection molding machine for a given mold, optimize cycle time, and reduce plastics material scrap
SolidWorks Plastics Advanced
SolidWorks Plastics Advanced gives you complete understanding of your tool design and the molding process, allowing you to model cooling systems, and analyze warp.
- Investigate and correct warping issues: Predict post-molding warpage, and take steps to modify the tool and molding parameters to correct, or create counter-deformed geometry to allow for warp
- Model and optimize cooling channels: Investigate different cooling strategies to produce high-quality parts as efficiently as possible, and completely understand the conditions within the mold tool
- Apply complex cooling conditions: Simulate advanced cooling strategies, like baffles, bubblers, and model conformal cooling around the part geometry
Continue to ping the blog; learn Plastics you will J
Post By John Hall
Another great new feature in SolidWorks 2014 is the ability to force all notes to be uppercase. We’ve all been in situations where we’ve forgotten to set the CAPS Lock while writing notes, only to have to re-write the note. With this new option, you can quickly toggle between the two without a problem.
You can do this on either individual notes just by selecting the note and setting the “All Uppercase” check-box in the note properties:
or by setting a document property to force all notes to always be uppercase
You can even set exceptions for anything that you need to display as lowercase, for items like units of measure.
SolidWorks 2013 introduced a new application called the SolidWorks Launcher that helps organize which version of SolidWorks opens the files. I mean, if we can open a 2013 file in 2012sp5 (a long-standing Customer request!) and have both 2012 and 2013 SolidWorks installed, then what should happen when we double-click the file in Windows Explorer? SolidWorks uses the Launcher to answer that question.
I'm bringing up this "old news" because sometimes, things don't go as planned and the Launcher isn't consulted when opening SolidWorks files from Windows Explorer. By default on a system with SolidWorks 2013 installed, SolidWorks file types should be associated to the Launcher (swshellfilelauncher.exe) and when opening files using double-click or right-click -> Open they should open in same SolidWorks session.
However, if the file types are associated directly to the SolidWorks 2013 (sldworks.exe), the files may open in separate SolidWorks sessions instead of the existing, open session. If that happens to you, check out this SolidWorks publication to correct the file associations:
SolidWorks Solution ID S-062896
Post By John Hall
Sometimes you want to add a second sheet to a drawing, and have the software use a separate template or something different than the original. For example, you may want a second sheet to contain a BOM, or sometimes you may want the first sheet to have an assembly, then subsequent sheets to show the parts that make up that assembly. In previous releases of SolidWorks, when adding the second sheet, you had to first add it, then specify the template by right-click on the background and specifying Properties.
New in 2014 there is an option for multiple sheets - you can very easily specify which template you want to use for sheet 2 and additional sheets that get added to the drawing. This is a quick and easy Document Properties setting; just go into Tools > Options > Document Properties > Drawing Sheets and you can specify the sheet format to use.
For a quick refresher on sheet formats and drawing templates, please see this article:SolidWorks Drawing Templates
Post By Jon Sorocki
Seeing is believing! What I am talking about is a spring in SolidWorks. While we can create motion with spring forces in SolidWorks, the spring itself is not modeled and doesn't move. To work around this obstacle, many users ask me how to model a spring that can be compressed or stretched in a SolidWorks animation. The answer is not too complex, but is definitely not orthodox.
What we are basically going to do is attach the path of a sweep to a face of another part.
First, let's model the spring. To make this coil, we are NOT going to use a helix curve. Instead, we will use a single sweep function with two sketches. Sketch a line on the front plane. It should start at the origin and go straight up. DO NOT give it a dimension. Rename this Sketch LENGTH. Sketch a circle on the front plane located somewhere off of the origin. I like to place a construction line from the center of the circle out to the right. I then pierce the free endpoint of the line to the LENGTH segment. You can make this line horizontal to guarantee a smooth sweep. Dimension the circle (gauge) and the distance from the origin (diameter).
Exit the sketch and rename it GAUGE. Choose Swept Boss/Base feature.
The profile will be the sketch GAUGE. The path will be the sketch LENGTH. Under options,choose Twist Along Path> Define by Turns. Set the turns to however many coils you need.This will create our spring. After the spring is finished, cut off sections on the top and bottom to make mating it easier.
To get the spring to move, place the spring into an Assembly. Mate the bottom of the spring to a face from another part (PLATE) with a coincident mate. I suggest mating planes of the coil and the PLATE to keep the spring from rotating. For this example, I have inserted a second instance of the PLATE to use as the motion driver. Save the assembly.
Edit the sketch LENGTH. Choose the free endpoint and another edge (circular, linear; it will not matter) from the 2nd PLATE within the assembly. Choose coincident relationship. Exit the sketch and exit edit part mode. (Yellow is spring preview. Pink highlight is the edge I selected.)
Now, move the 2nd PLATE up. Press rebuild (ctrl+B). Move the face of the body down. Press rebuild. You should see your spring change in height.
With the relation is set up; let us get the animation going! Create a new animation through Motion Study.
Move the time bar to 2 seconds. Drag the PLATE up.
A key should be placed for you on the timeline. Move the timebar to 4 seconds. Drag the PLATE down. Another key is placed for you.
Press Play from Start. You should see the spring move dynamically!