Creating SolidWorks Library Features From Scratch

June 17th, 2015

6 Easy Steps to Create SOLIDWORKS Library Features From Scratch

Creating Library Features from scratch is a VERY valuable technique to know. It can save you tons of time when you have “common features” that you want to reuse over and over again.
In this case let’s say we have a drafted, filleted, pocket that we are tired of creating over and over every day. (Fig. 1) We would like to “capture” this feature into the Design Library so that we can just Drag & Drop it into any model.

FIG1

1. MODEL THE FEATURE ONE TIME…

Yes. You do actually have to build it one time. When you do, consider if you want it to be “locked down” with some locating dimensions, or if you want it to remain “free” to position anywhere. If you do add dimensions to locate the feature (from the side and bottom edges in this case) then you are laying an extra requirement on the end user that they will have to identify those references (edges in this case) when they use it. This action is really repairing the dangling relation/dimension that comes in with the feature.

 

2. (optional) RENAME THE IMPORTANT DIMENSIONS TO LOGICAL NAMES…

This step is totally optional, but sure does make the part a lot more user friendly. If you just leave everything named “D1@Sketch3” and “D4@Cut-Extrude2” that isn’t going to make a lot of sense to anyone who goes to use this Library Feature.  If you right click on the Annotations folder in the Feature Tree and turn on “Show Feature Dimensions” (Fig. 2) this will display ALL of your part dimensions on the screen. Then if you also turn on “view dimension names” from the heads up view toolbar (Fig. 3), you can see the names that were auto assigned. Now you can just select a dimension and over in the Property Manager give it a new name. Or you can double click a dimension and change its name right there. (Fig. 4) You of course only need to worry about renaming the dimensions that you are actually going to use in the library feature. In this example we wouldn’t need to worry about renaming any of the dimensions in the big block. Only those in the “pocket” features.

FIG2  FIG3

 

FIG4

 

3. (optional) CHANGE THE COLOR OF THE ACTUAL FEATURE(s), AND ORIENT…

In the Feature Tree, Ctrl+select the features that make up the library feature you want to create. After you let go of the Ctrl key, on the pop up toolbar will be an appearance icon (color ball). (Fig. 5) Use this to change the FEATURES to something that stands out. You could also change the rest of the part to something like gray or white. This is just going to make the thumbnail graphic show better in the Design Library. Next you would want to orient your model to however you want the thumbnail graphic in the Design Library to look. However, there is a setting you most likely want to turn OFF. It is Document Properties—Image Quality (Fig. 6)

FIG5

FIG6

 

4. ADD TO LIBRARY…

Open up the Design Library in the Task Pane and navigate to the folder you want to store your new library feature in. Hit the “Add To Library” button at the top. (Fig. 7) In the property manager that comes up on the left, under “Items To Add” (Fig. 8), BE SURE to select which features you want included in the Library Feature! (use the flyout feature tree). For example in this model we would select everything EXCEPT the first feature (the big block that we cut the pocket into). If you included that block then it would also get inserted when you used the Library Feature rather than just the pocket with the fillets. A lot of people miss this step. By the way, you could of course PRE-select the features in the feature tree BEFORE hitting the “Add To Library” button if you wanted… Hit OK to finish adding the features to the library.

FIG7     FIG8

 

5. ORGANIZE/CLEAN UP THE LIBRARY FEATURE…

You should now be in a “.sldlfp” (library feature part) file now. Look in the Feature Tree. There should be green “L”s on all of the features that you intended to be included in the library feature. (Fig. 9) The library feature is really ready to use, but there is some “clean up” work that should be done in the file first. Open up the “REFERENCES” and “DIMENSIONS” folders in the Feature Tree. (Fig. 10) The References folder shows what the user will have to “satisfy” when using the feature. In this example the user will drag & drop the feature onto a face to satisfy the Placement Plane, and then they will select two edges to position the feature. These two edges are required because we DID put positioning dimensions to some edges of the block in the original part. If we had left the original feature “free” to move, we would not have this requirement in the Library Feature. In the Dimensions folder, drag any dimensions that are considered “locating dimensions” into the Locating Dimensions folder (i.e. the two dimensions from the edges of the block). By default when the library feature gets used, any of the other dimensions listed in the Dimensions folder will be able to be modified as the feature is placed. This is very nice to be able to modify the feature on the fly on a case by case basis. However, if you want to lock the user out of being able to modify certain (or all) of the dimensions of the feature, drag those dimensions into the Internal Dimensions folder. In our example we have locked the user out of being able to change the Draft Angle and the Corner Radius of the pocket. (Fig. 10)
Now Save the .sldlfp file one more time, and then close all open files.

FIG9     FIG10

 

6. YOU’RE DONE! TRY USING YOUR LIBRARY FEATURE !!!

Have fun creating an infinite number of Drag&Drop features in your library to save you tons of time!

 

Have you every used Library Feature?  Let me know in the comments why you used it or if you wish you knew about it before now. For more  SOLIDWORKS Tips and Tricks follow us on Twitter for weekly Tech Tips.

 

Randy Simmons

Application Engineer, CSWP 3DVision Technologies

Right Sketch, Wrong Sketch Plane

June 10th, 2015

How many times have you created a sketch and then figured out that it’s on the wrong sketch plane or face.  Even after all the years that I have being using SOLIDWORKS I still do that.  You have the ability to move a sketch to a different plane/face with about 3 mouse clicks.

First you need to be out of the sketch.  You don’t want to be editing anything.

Find the sketch that you want to move.  The sketch could be consumed by a feature…it doesn’t matter.  Then you can right mouse click on it.  This will cause the in-context property manager to appear.  The great thing is that it’s right next to your mouse.

You will want to choose the ‘Edit Sketch Plane’ option.  This allows you to move it to a different face or plane.  It is the icon that looks like a plane with a hand pointing to it.  It is the second icon.

Edit Sketch Plane

 

You can also get to the option under Edit, Sketch Plane.  It’s the same feature as on the in context tool bar.

It then asks you where you want to place the sketch.  You can choose either a different face or a reference plane.  The face that you choose could be parallel to the original one, perpendicular, or angled.  It doesn’t matter where it is.

ESP Dialog Box

It is possible that you will get a message box that says something about moving it to a different face will cause dimensions or the relations to fail.  That happens when the edge you were originally referencing cannot be found.  I would suggest just choose to delete the item and add the dimension/relation back in.

Have you every used ‘Edit Sketch Plane’?  Let me know in the comments why you used it or if you wish you knew about it before now.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

PCBWorks Now Available

June 9th, 2015

Every engineer knows the pitfalls that await when the electrical and mechanical sides of our design process fail to integrate their workflows and design data. But do we also understand all of the underlying costs associated with these design process failures? With the rising need for connected design experiences, we are at a unique juncture in the evolution of our design tools where collaboration features are becoming a daily necessity. As engineers strive to strike the perfect balance of aesthetic emotion and electronic functionality a design process that rewards experimentation, not penalizes experimentation, is surely needed.

The True Costs

It’s rare these days to find a mechanical design that exists in isolation with no PCB counterpart. As connected as the physical customer experience is, our ECAD/MCAD design collaboration process is commonly fragmented and separate, with both sides vying for control and struggling to communicate. And we all know what this leads to:

  • Missed time to market and budgets with design revisions slipping through the cracks and prototype costs skyrocketing from failed communication processes.
  • Wasted time and productivity with designers having to manage multiple revisions that could have been solved the first time with a properly implemented collaboration system.
  • Product experiences that are compromised during the design phase based on budget and time constraints vs. being iterated to perfection.

Tangible Pain

We engineers always love concrete data, so consider this the next time you are facing the potentiality of a failed design process:

  • The average company creating a moderately complex PCB requires 14.1 physical prototypes, at an average cost of $8,929 per prototype. Can your budget really afford numerous prototypes that fail to fit your mechanical enclosure because of a communication breakdown in the design phase?
  • On average, Engineering Change Orders (ECOs) cost $1,984 to implement during development, and $10,625 once a design has been released to manufacturing. How many ECOs has your company generated in the last year because your ECAD/MCAD designers weren’t on the same page?

A New Reality for Collaboration

Introducing a new PCB design tool specifically made for direct integration with SolidWorks® and a mechanical designers existing workflow – PCBWorks.

When we looked at the traditional design environment in several companies, what we found is mechanical designers leading the workflow process, with the mechanical enclosure being the final determinant for how a design would come to completion.

Changing the mechanical designer’s tool would lead to a disruption in this traditional structure, and the weak link was clearly the PCB design tool being used that had no intelligent data connection with the mechanical environment.

PCBWorks solves all of the old problems of design collaboration, incorporating a number of powerful features that intelligently link design data to keep both design teams operating at their highest peak of efficiency. With PCBWorks, you can:

  • Actively make changes to component placement, board shape, and mounting holes on your PCB directly in your SolidWorks® environment, syncing data with PCBWorks easily with managed ECOs.
  • Ensure that your design data is as accurate as possible by using SolidWorks® native Parasolid file format directly in PCBWorks. By using native lossless files instead of error-prone translations, Parasolid provides the most accurate representation of your design intent and keeps your mechanical and electrical data in sync.
  • Gain an even greater degree of control over your PCB design process with access to copper traces from your board designs. Native Parasolid board data provides a new-level of analysis capabilities directly within SolidWorks® with thermal, vibration and other simulations.

That’s just a small sampling of everything that’s possible in PCBWorks for design collaboration. And with over 25 years of experience in PCB design, you can be assured that PCBWorks includes all of the necessary power needed to easily handle today’s electronic designs. Check out all the features in PCBWorks at http://www.3dvision.com/solidworks/partner-products  and see what’s possible for your design collaboration process.PCBWorks

3DVision Technologies

Your destination for design and manufacturing technology

DriveWorks for Sheet Scales

June 5th, 2015

If the overall size of your models change significantly, there is a good chance you will need DriveWorks to change your drawing sheet scales to keep your model looking nice on the sheet.

Imagine this is my drawing. Let’s say the height of my part does not change much, but my length (which is currently 100 in the model master) can change significantly.

DriveWorks Drawing

 

DriveWorks (Pro and Solo) gives us two sheet properties that we can use to drive the sheet scale:

Rules

If your company does not have standards on view scale requirements, the value of these two properties is rather simple. Set the numerator to always equal 1 and the denominator is a ratio of the new length to the old length times the current master sheet scale. So if my current sheet scale (in this example) is 1:5, my denominator rule would be (New length)/100*5. Making your rules look something like this:

PopulatedRules

Now your drawing will automatically scale up or down depending on the length of the part. (Make sure your views are all using the sheet scale Drive Works sheetscale…or you can create rules for the individual views too.) Granted, it makes for some non-traditional sheet scale values (My drafting teacher would die if I put “1:3.76″ on in the title block, I usually just put “NOT TO SCALE”) but nobody puts calipers on drawings anymore anyway.

Cake.

…but what if your company is still using old standards that demand scales such as these:

Full size: 1:1
Enlargement scales: 2:1, 5:1, 10:1, 20:1, 50:1
Reduction scales: 1:2, 1:5, 1:10, 1:20, 1:50, 1:100, 1:200, 1:500, 1:1000, 1:2000, 1:5000, 1:10000

First, try to get an exception. (Why would DriveWorks created drawings have to follow this antiquated rule?) If you can’t get an exception, make a lookup table in DriveWorks.

DriveWorks Factors

Call the table something clever like “ScaleFactors”

First lets look at times when we want a reduction scale. (The numerator = 1). In these cases, we usually “round up” our numerator to the next larger scale factor (it is better for the views to be too small rather than being too big -and go off the page)

Now my previous denominator rule would look like this:

DMin(DwLookupScaleFactors,1,">=" & (New length)/100*5)

“DwLookUpScaleFactors” is the name of my table, I’m looking in the first column of that table, then finding the smallest number (DMin) that is greater or equal to the scale ratio that I calculated earlier. (So if my length is 100, DMin returns 5. If my length is 101, DMin returns 10)

In cases where we need an enlargement scale, the logic is the same except the denominator is = 1 and the numerator rule looks very much like the denominator rule above except you need to take the inverse of the ratio.

If you sometimes have a enlargement scale and sometimes have a reduction scale, an if/then statement is all you need. In pseudo code your denominator would say:

if("Enlargement scale",DMin(DwLookupScaleFactors,1,">=" & (New length)/100*5),1)

and your numerator would be

if("Enlargement scale",1,DMin(DwLookupScaleFactors,1,">=" & 100/(New length*5)) (Notice I took the inverse of the ratio)

Not very hard, but see why I wanted you to get rid of the scale factor standard?!

Questions about Driveworks or drawing sheet scales? Use the comment section below.

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Pack and Go Now Available for Flow Results

June 3rd, 2015

Pack and Go Now Available in SolidWorks Flow Simulation

Pack and Go has been a staple in SolidWorks functionality for years. It allows a SolidWorks user to package SolidWorks  files such as Assemblies, Parts, and Drawings into a new folder location, or a Zipped file.  Pack and Go can keep the current file structure of folders and sub folders, or flatten to one folder.  This allows a user to make back ups of their work, or transfer files to others easily.  You can rename the new saved files individually or globally with a suffix or prefix creating a new file set.  The user does not loose custom appearances decals or scenes saving time and work when copying the files.  Toolbox components can also be included in the Pack and Go.

SolidWorks Simulation files have always been able to be included with the Pack and Go, However New for 2015 SolidWorks Flow Simulation can now add results files (.fld) to a Pack and Go.  This added functionality allows a user to quickly roundup all the important files needed to transfer, or store their design.  Simply select the Pack and Go option from the file menu. Choose the “Include Simulation Results” check box, and proceed like normal.  Please note that with the Flow Results included the Pack and Go .zip file will be large in size.

Pack and Go

Pack and Go has always made it easy to accumulate all the important files to transfer or store.  Now in 2015 Flow results are added to this great functionality. Lets us know through the blog comments how this functionality has helped you in your daily engineering tasks.  Pack and Go will continue to improve and add functionality as it matures.  Users like you help shape how the product behaves and what new functionality is added.  keep up the good work.  It has been requested for a while and we finally have Flow Results included with Pack and Go.

 

Robert Warren

Elite Application Engineer CAE Technical Specialist 3DVision Technologies

2015 Manny Award Winners

May 29th, 2015

3DVision Technologies Customers Win Multiple Manny Awards

Congratulations to all the 3DVision Technologies customers who were named 2015 Manny Award winners. The Manny Awards are committed to recognizing the manufacturing industry’s greatest accomplishments, and in doing so will honor local companies for their innovation and best practices.  Winners of this prestigious award have exemplified accomplishments in areas such as: product innovation, e-business, supply-chain management, employee safety, systems/process innovation, global business, technology transfer and quality control.

We are proud to announce we had customers win in multiple categories including:

Best Place to Work

Polymet Corporation – A world class manufacturer of high performance welding, hardfacing, and thermal spray wire,

Richards Industries – The parent company of several distinct industrial product lines: regulators, control valves, team traps, steam specialty equipment, paper products, tire and rubber, machinery and electrical equipment, transportation equipment and energy industries.

Biggest Breakthrough

SugarCreek – A diversified, innovative and extraordinarily flexible food manufacturer with five – soon to be six – major facilities. Providing a wide-ranging, value-added assortment of raw and fully-cooked products for domestic and international customers across all channels of trade.

New Product Development/Innovation

Arnold Gauge Company, Inc. –  They provide the world’s finest “in-process” measurement solutions. Striving to utilize the latest in people, process, design, and technology to provide you with the finest measurement solutions possible.

Deceuninck North America – A fully integrated design, compounding, tooling, and extrusion company that produces vinyl window and door systems and composite applications for the building and construction industry.

Top Growth

Fecon – The Industry leader in forestry mulching attachments.

Intelligrated – A leading North American-based, single-source provider of intelligent automated material handling solutions that drive distribution and fulfillment productivity for retailers, manufacturers and logistics providers around the world.

Mubea – Using new lightweight construction technologies, new materials and processing methods, they create innovative solutions for the construction of lighter vehicles.

Hall of Fame Leadership Award

Gary Heiman, President & CEO, Standard Textile –  Leveraging textile design, manufacturing and laundry expertise, as well as their global infrastructure, they serve customers in the healthcare, hospitality, decorative products and industrial apparel marketplaces worldwide.

Want to attend the 2015  Manny Awards?

The 2015 Manny Awards will take place Wednesday, June 17th at the Sharonville Convention Center. Starting at 5:45pm with a Networking and Cocktail hour. Dinner and the awards presentation will begin at 6:45pm. The RSVP Deadline is Thursday, June 11th.  To RSVP and purchase your tickets for the event click here.

 

Manny Awards

Cody Markham

Assistant Marketing Manager 3DVision Technologies

3D ContentCentral: Get Those Models for Free

May 28th, 2015

Most companies I work with use purchased components and want to add them into their assemblies.  So how do you get the solid models?  You might contact the company for the model or just model it yourself.  Well you could download the models for free without contacting anyone by using 3DContent Central.

3D ContentCentral Logo

3D ContentCentral (3DCC) is a free service for users to download solid models.  How is this different than other similar sites?  This is a Dassault Systemes site and the models are not just from users.  You have the ability to download models that other users have modeled but you also have the option to download from certified suppliers.

Suppliers can upload their models from their catalog to allow consumers to download them for free.  This way you can add it to your assemblies and have the BOM show the true items to be assembled.

3D ContentCentral BOM

There is also integration into your SOLIDWORKS interface.  If you open the Design Library, you will see it on the right side.  When you click on it, it will take you to the website allowing you to download the files.

3D ContentCentral  Integration

Many of the files allow you to configure them before you download.  So you can choose a different color, different size, etc.  You can also choose what format you want to download the file in.

3D ContentCentral Configure

How many suppliers are on 3D ContentCentral?  I just counted 840 which are from all over the world.  You can search for a specific supplier or find them in the global list.

So what if you want a model from a supplier but they aren’t on 3DCC?  You have the ability to request the content.  You can make the request to have a member of the 3D ContentCentral community model it.  Or you can request that a supplier be added to 3DCC.

3D ContentCentral Request

3D ContentCentral is going through a website redesign.  They are changing the interface, adding a new eDrawings viewer which will be available in many browsers/mobile, and an improved searching tool.  The viewer will allow you to rotate, section, and shade the models so you know what you are downloading.

3D ContentCentral preview

Check it out here: Beta 3D ContentCentral

3D ContentCentral Interface

I have used this site many times and have suggested users check it out.  There are over 1.3 million members who have used 3DCC.  Are you one of them?

Let me know in the comments below if you’ve used it and what you think.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

Store Project Constants in EPDM Folder Cards

May 22nd, 2015

With nearly every design, you’ll have a few variables that nearly every decision hinges off of… working height, conveyor height, cycle time, etc. These values always seem to change, forcing a lot of updates through out your designs.

There are several ways you can link your SOLIDWORKS models to these constants. The most common methods involve creating relationships between your parts and other files [“Layout sketches”, “Skeleton Sketches”, “Phantom Parts”] these parts get inserted into all of your assemblies. It works but can make quite a spiderweb of relationships. I am becoming a fan of storing project constants in the SOLIDWORKS Enterprise PDM’s folder card. Then I link my dimensions to these folder card values through SOLIDWORKS equations.

Let’s imagine I am designing a table and I always want my table height to always be 3″ less than the conveyor height. First I’ll store the conveyor height in the project’s folder card.

FolderCard2

These constants also need to exist on the SOLIDWORKS file card.

Folder Card SWCard

Make sure you have the file card control to inherit information from the folder card. So that as we add files to the project the file’s data card will get its information from the folder card.

Folder Card Inherit

The variable needs to be pushed into the file’s custom properties

Folder Card VariableLink

SOLIDWORKS equations can use file properties as part of their arguments:

Folder Card LinktoProperies

Below you see that I am taking the “ConveyorHeight” and subtracting “3” from its value. If the “ConveyorHeight” ever changes, the dimension named “TableHeight@Boss-Extrude2″ will update automatically.

Folder Card Evaluated

Here is another cool thought. Now not only if the conveyor height changes for this project will all my parts update (using EPDM’s Update function), but if I copy any of these parts into another project and have “Default overwrites” turned on for the card variable, these parts will automatically update to their new project’s values as they get copied from one project to another.

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

3D Printed Lithophane

May 19th, 2015

A lithophane is defined as an etched or molded artwork in a thin translucent material that can only be seen clearly when lit from the back. They have been around for a thousand years dating back to ancient China. Our 3D Printing Application Engineer, Jeremy Marvin, added a modern touch to this ancient art form. He printed his daughter Gabrielle “Gabby” on a Fortus 400 using ASA plastics. See the amazing results below.

Flat View of 3D Printed Lithophane

3D Printed Lithophane

 

3D Printed Lithophane Without Light

3D Printed Lithophane

 

3D Printed Lithophane with Light

3D Printed Lithophane

Cody Markham

Assistant Marketing Manager 3DVision Technologies

STL Output Settings for CAD

May 15th, 2015

Last fall I switched responsibilities here at 3DVision.  I moved from the SOLIDWORKS side of our business to 3D Printing.  Some of our readers may recall chatting with me on Technical Support or sitting in one of my training classes.  For my first “official” blog post I thought it might be good to mix both worlds – CAD and 3D Printing.

CAD comes into play when we think about what we need to print.  Currently, the industry standard file format for 3D Printing is the STL (Standard Tessellation Language) file.  All major CAD packages can save or export in the STL format, including SOLIDWORKS.  Simply click File-Save As-STL.  Once the STL file type has been selected you’ll notice an options button appears.  Clicking this options button shows you all the settings we can change regarding the STL File itself.

 

STL

Quick Tips when setting up your STL Output

1.  Use the Binary option to save disk space, it reduces the file size by a ratio of 6:1.

2.  The STL itself is unitless.  SOLIDWORKS will output in the specified units, no matter what unit we use in our model.  When we bring the model into our 3D Printing software, we’ll need to specify the units used.  If the parts come in really big or small, the software will ask you to confirm.

3.  Stratasys recommends a Deviation tolerance of .001″-.012″ [.03mm-.3mm] I generally set the resolution to Custom and use .0005″ which is a touch smaller than they recommend. The files tend to grow very fast when you get down much smaller than that.  The bigger the file the longer it takes to process in the 3D Printer software.  [I have a model from a customer that was 750mb and took 30 hours to process.  We need to strike a balance between getting a high tolerance part and keeping file size/processing time down.]

4.  Stratasys recommends an angle tolerance of 5-10°.  The default in SOLIDWORKS is 10° so I leave this alone.

 

Below is a small example explaining the Deviation (chordal tolerance) and the Angular tolerance.  This is the max difference allowed between the faceted surface and the SOLIDWORKS Model.

STL

We can’t print a model better than the STL, so it is always good to check the options before saving the model, and verify the STL looks good before processing.

STL

 

Keep an eye out for future blog posts regarding 3D Printing and be sure to comment below. I’m currently working on a multiple part blog regarding part orientation so stay tuned.

Jeremy Marvin

Application Engineer - 3D Printing 3DVision Technologies

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