Archive for August, 2011

Simplified (McMaster-Carr) Parts in Assemblies

Wednesday, August 31st, 2011

The following golden rule applies to 99% of you out there…

Never include fasteners with modeled threads in your assemblies.

This is the reason the SolidWorks toolbox comes with three options for thread display when inserting fasteners into your assemblies: Simplified, Cosmetic, and Schematic.  The popular and recommended choice is ‘Cosmetic‘ – a healthy combination of detail and efficiency.

toolbox-thread-options

There are quite a few factors that can contribute to clunky and inefficient assembly models, but two very obvious culprits are the quantity/complexity of features and surfaces.  You can apply this concept to any type of model, but modeled threads are a perfect example to discuss both of these slow downs.  Though there are times when it makes sense to model threads within a part file, it’s rare that those threads are needed within an assembly file.

One of the coolest things about McMaster-Carr (besides their same day delivery of just about anything you can ever dream of) is that they offer 3D models of a majority of their products in a native SolidWorks file (i.e. feature tree, dimensions, and relations are included).  McMaster-Carr customers with SolidWorks have a huge advantage over the rest, because they’ll be able to quickly edit these files however they’d like.  Here’s an example…

  • Download a 1” long ¼-20 SHCS from McMaster-Carr and notice that the part comes fully equipped with modeled threads.
  • Click Tools > Feature Statistics and note the 0.80 second calculated rebuild time.
  • Right mouse button (RMB) the “Cut-Sweep1” feature, and select “Configure Feature” from the menu.
  • Create a “Simplified” configuration with the thread cut feature suppressed.

fastener-detail

  • Run the Feature Statistics tool one more time and you’ll see a 0.15 second rebuild time.Just by removing one feature, we managed to cut the rebuild time to less than a fifth of what it was.  This goes a very long way inside an assembly where many of these fasteners can exist.

Obviously, you can make “Simplified” configurations for any type of model (not just threaded fasteners).  You can suppress any type of feature that is not required to be present in the assembly (complex features, fillets, chamfers, etc.).  This is a great way to speed up large assembly performance.  All you have to do is activate the “Simplified” configuration of all the part files within an assembly.  “How?”, you might ask…

  • Click File > Open within SolidWorks and browse to an assembly file.
  • Before opening it, click the “Advanced” check box.
  • When you click the “Open” button, select the following options on the pop-up menu.

simplified-configurationOnce you click OK, SolidWorks will find any part within the assembly (regardless of the levels of sub-assemblies) that has a “Simplified” configuration and activate it.  Simple (no pun intended)!  Why not create a simplified configuration for every part file?

Jordan Tadic

Certified Elite Application Engineer 3DVision Technologies

Free Weldment Profiles!

Tuesday, August 30th, 2011

Back in January, when Jordan Tadic published his cut lumber library for use as weldment profiles, the CAD community went crazy! For a brief period of time there was concern that we may need to get a larger server to help handle the additional page requests.

Did you know you can get weldment profiles from SolidWorks? – significantly more than the few you get by default when you install SolidWorks.

Go to the design library, expand “SolidWorks Content” and browse for all kinds of free goodies to make your life easier!

DownloadProfiles

(You’ll also find drawing blocks, standard parts and Unistruts here too.)

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Model Aircraft Control Surface Spacing and SolidWorks Flow Simulation

Saturday, August 27th, 2011

June 2011 AMA (Academy of Model Aeronautics) Model Aviation magazine had an interesting article Titled “Two of the Big Five model misadjustments” written by Dean Pappas. The two misadjustments were Hinge Gap, and Lateral Balance.

The article caught my attention specifically due to the “flow” diagrams drawn in the article explaining airflow over the wing section and aileron control surface. In the below diagram, taken from the article, Dean explains three cases of air flow relative to a control surface.

  1. Clean airflow at the neutral control surface desired for level flight.
  2. When up or down direction is applied to the control surface the air opposite the control surface direction of travel redirects the flow to reattach. This case shows a tight fit between control surface and main structure.
  3. Hinge gaps allow high-pressure air to leak from one side to the other. This weakens airflow on top of control surface partially destroying the bottom airflows ability to rejoin it. The result is poor control surface response during slow speeds.
AMA Article Diagram

AMA Article Diagram

According to the article ”The high pressure on top, as shown would leak through, given a chance. That chance would be a gap in the elevator and control surface. The result is a flat sheet of air that squirts through the gap and distorts the outside of the hinge line. This reduces the effectiveness of the elevator and creates extra drag.”

This section piqued my interest as the hinge gap shown is very large, probably for demonstration purposes. Being an avid RC aircraft modeler I suspected that the small gaps I have in my personal aircraft’s control surfaces may not cause this affect. My hypothesis is that a very large unrealistic gap will cause this affect however using standard hinge techniques this affect will not be as dramatic as the article states. According to the article large hinge gaps can be sealed with strips of MonoKote covering resolving the problem. MonoKote is a heat shrink Mylar covering that is a standard in RC Aircraft construction.

This blogs purpose is to investigate the hinge gap spacing required to cause an airflow disturbance and air leak through the gap area.

Before we get into the model specifics let’s talk a little about aircraft wing terminology. Below is a diagram explaining common wing dimensions and terminology. The chord length is the distance from the leading edge of the wing or elevator to the trailing edge. The model used in this Flow Analysis is a 5.5″ main wing chord. 0.5″ of the chord is the control surface . The airfoil is symmetrical so the upper and lower camber are equal. The model consists of an extruded wing section with one hinge placed in the middle of the wing.

Airfoil.svg

Three hinge types are standard in the RC modeling community. All hinges are typically spaced evenly across the control surface.

  • Standard plastic barrel hinge comprised of two halves held together with a pin. The hinge is typically screwed or glued into place with the barrel tight against both mating sections. Hinges are typically 0.25″-0.5″ wide by 0.5-1″ total length. The barrel typically ranges from 0.0625″-0.125″ in diameter.
  • CA hinges are flat woven wicking material that is inserted into a slot cut in the components. No or little gap is present with this style hinge. CA or Cyanoacrylate glue is used to wick through the hinge and bond with the hinged components.
  • MonoKote hinges are seldom used in modeling except for small aircraft. The MonoKote hinge is typically a strip of MonoKote that is applied to the top and bottom of the hinge area.

SolidWorks Flow simulation was used to investigate the control surface configurations of four models.

  1. A base line neutral control surface position using a no gap CA hinge Type.
  2. Upward deflected control surface using a no gap CA hinge type.
  3. Upward deflected control surface using a Standard plastic hinge with an 0.0625″ barrel diameter.
  4. Upward deflected control surface using a CA Hinge and gap of 0.25″

All configurations have a 10 ft/second flow rate and a 0 degree angle of attack. The flow analysis was an external flow problem. A localized mesh control was used for each run to capture refined accurate results across the model boundary. All other default conditions were used for the flow setup.

Mesh

Note All plots show a Pressure cut plot and Velocity Flow Trajectories.

Results:

  • The base line model showed a symmetrical pressure on either side of the wing at 14.6 psi and a hinge crossing velocity of 16.45 ft/sec. This is expected results for the area section, hinge, and aileron placement.

Neutral Velocity and Pressure

  • Flow Run Two shows a higher pressure on top of the aileron of 14.696 psi and a lower pressure on the bottom of 14.694 psi. The flow velocity across the top of the control surface drops to 5.9 ft/sec while the bottom speeds up to 11.2 ft/sec. As the article states the air “bends” to re attach to the flow at the trailing edge. This results in a turbulence on the bottom of the control surface aiding in the force of the air on the top of the control surface to push the trailing edge down.

Aileron Up CA Hinge

YouTube Preview Image
  • Flow Run Three demonstrates the 0.0625″ barrel hinge gap and the resulting air flow. The run does show airflow across the gap boundary, however probing the area the velocity in this gap is zero. The flow does extend past the wing trailing edge longer than the non-gap position, however the flow does fully rejoin. The same recirculation under the control surface is seen . The pressure on the end of control surface is however higher at 14.699 psi and lower on the bottom at 14.692 psi. The results show negligible flow through the gap and under most circumstances(slow flight) should not cause loss of control due to bleed through.

Aileron Up 00625 Gap

YouTube Preview Image
  • Run Four had the largest gap similar to the gap in the article’s diagram. The flow results show airflow across the gap boundary and a velocity of the airflow in the gap of 3 ft/sec. The flow does extend past the wing trailing edge longer than the non-gap position and does not rejoin. The recirculation does cause a pressure equalization under and over the control surface. Loss of control surface effectiveness would occur in this scenario.

Aileron Up 025 Hinge Gap

YouTube Preview Image

Conclusions: The article is correct to a point. The gap shown in his diagram would cause a control surface loss of effectiveness, however the gap is way too large to be considered realistic. Most experienced modelers know common practice is to get as tight of a fit between control surface and structure be it a wing, elevator, or rudder. A large gap is not only detrimental but is also unsightly and most modelers avoid them for the aesthetic reasons alone. If a modeler sticks to the new CA hinge or follows correct installation practice for a plastic hinge they will be alright in their flying endeavors.

Robert Warren

Elite Application Engineer CAE Technical Specialist 3DVision Technologies

Color Selection in DriveWorks Solo

Thursday, August 25th, 2011

I’ve done some research. Even though all pictures from 1903 are in black and white, there were actually eight colors back then! Red, yellow, blue, green, orange, brown, purple, and black. If life would have stayed like that everything would be simpler.

Sadly, someone let the hippies have their way, and now there are many more colors. Most I have no idea what they look like by name alone. Thus if you give me a simple list of colors it has little value to me.

My challenge was that I wanted to be able to let my user choose between a very large list of colors in DriveWorks Solo.

SimpleList

Nice, pretty, but what color is sienna?

Here was my solution.

I set the background color property of the list control to be equal to the color chosen. The default background color for all controls is white. (I know that color!)

Properties

See that little gray dot next to the color in the image above? That means the property is static and cannot be changed by a rule, but if you double click on the gray dot, you can create a rule to connect the background color to the color chosen. Like this:

WithRule

Now when you change the color in the list box, the background color will dynamically change!

WithColor

This works pretty good, unless the user chooses black, then you can’t see the text.

A second option would be to add a little picture box near your drop down, and just like before, link the background color to the chosen color value.

Background

Parting tip: This doesn’t work for every color ever named. Ensure your drop list contains only colors listed in the DriveWorks Solo color web tab –even DriveWorks knows only a finite number of colors.

WebTab

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

EPDM Fundamentals

Tuesday, August 23rd, 2011

Looking for a way to convince your manager that you need PDM but you know he  only responds to pretty pictures and peppy music?

It’s intervention time.

Tell him there are doughnuts in the conference room, get Big Larry to stand by the door to keep him inside and play this video on the projector. It’s only two minutes long, he should be able to pay attention as long as you ensure nothing shiny is in the room.

thumbsup

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Update Properties from BOM

Monday, August 22nd, 2011

Here’s a tip that you might not know about.  You can update component/sub-assembly properties from a Bill of Materials.  Why would you want to do this?  Well in case you forgot to add the property when you created the component, maybe you didn’t know what it was at that time, or you see you filled out the wrong information.  Now you can add or change the property without opening it up.

All you need to do is double click in the cell of the BOM and then you will get a message about keeping or breaking the link.

Link

You will have to choose “Keep Link” to update the property.  Now whatever you type in the cell will show up in the component’s properties.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

EDSM, What are SolidWorks User Groups Like?

Friday, August 19th, 2011

Mail Call!

Dear Engineering Data Specialist Man, I have been wondering about attending a SolidWorks user group meeting. What are they like?

Peyton M, Indianapolis Indiana.

That is a good question Peyton, as a matter of fact I was in your town last night for a user group meeting. Here is how it went:

After we went around the room introducing ourselves, Mike and Jon Caliguri gave a presentation on Delcam. This was the first time I had seen their SolidWorks interface, and I liked it. The integration was great -it was hard to tell where SolidWorks ended and Delcam started. It looked easy to use and passed my PDM test. [For a CAM package to pass my PDM test, it must be possible to store CAM data without having to get write access to the part.] Delcam solves this issue by putting the part into a blank assembly and storing the CAM data in the assembly. As a second bonus to this method if you save that assembly in SolidWorks Enterprise PDM, EPDM would see that the part is inside of that assembly, thus the two files would be automatically linked via the “Contains” and “Where Used” functions.

Delcam

Next came Don Hope‘s favorite part of the meeting. Dinner. 1. The Teppanyaki Grill easily had the largest selection of any Chinese buffet I have seen, and the food was very good too. (I gave it five out five of bellies.)  2. The price was right because SolidWorks picked up the tab.

During dinner I tried out some of my new dinner jokes. Chris Snider said they were funny, but his body language seemed to say else-wise.

Notfunny

Much to the surprise of Lisa Van Giesen, I provided the second program. My topic was on DriveWorks. Since everyone in the room had access to DriveWorksXpress, I spent most of my time on it. However we did have enough time to discuss some of the features of Driveworks Solo and Professional.

After my presentation, there was a little time left for some tips and tricks. Three members brought up special CAD challenges they were having, and as a group we were able to come up with satisfying solutions for two of them.

Lastly, door prizes were passed out, a song was sung and we went home.

gettingdoorprizes

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Central Indiana SolidWorks User Group Meeting – August 18 – DriveWorks Demonstration

Thursday, August 18th, 2011

Attended a SolidWorks User Group (SWUG) meeting recently? If not, you are missing out – not only on free food, but a great chance to network with your SolidWorks peers and learn some new things about SolidWorks that could make you a lot more productive at work.

If you live in the Central Indiana region, you can plan on attending the CISWUG meeting that is scheduled for this Thursday, August 18th at 5pm.

To sign up, please RSVP with Peter Fischer by emailing him at info@indianasolidworks.org. Please put “Reservation August 18th meeting” in the subject line.

The details are below. Hope to see you there!

Date: August 18
Location: Teppanyaki Grill – 9701 East Washington St, Indianapolis, IN (South end of Cherry Tree Shopping Center)
Time: 4:30pm – Registration and networking. Meeting starts at 5:00pm
Agenda:

  • General Meeting
  • Followed by Jon Caliguri, Design and Software International. “Integrating SolidWorks CAD to CAM”
  • Dinner: (Sponsored by SWUG Corporate)
  • Technical Presentation:   Jeff Sweeney, 3D Vision “DriveWorks 2011″ A powerful tool for multiple version of same-as-but products, and it comes free with every seat of SolidWorks. 
  • Followed by SolidWorks ”Tips & Tricks”. All participants are invited to bring their ideas.
  • Door Prizes: 7:30pm ish.

 

Chris Snider

Application Engineer, CSWE 3DVision Technologies

eDrawings App on an iPad/Android???

Wednesday, August 17th, 2011

Let’s face it, the world is fast paced and having data at our fingertips can be the lifeblood of our businesses. Enter the Tablet! Often times heavy computing is not necessary when we are “On-The-Go.” We can whip out an iPad or Android Tablet and effectively communicate business needs to our customers, and we don’t have to wait for the tablet to boot up, login, prepare our desktop, connect to our servers, yada-yada. The information is literally a swipe or a tap away.

eDrawings is a very effective product from Dassault Systemes SolidWorks that allows you to communicate your designs with customers, without having to transfer heavy files via email or even FTP sites. So, it seems perfectly suited to have an eDrawings App for tablets.

Ever since the first iPad hit the market I have been getting calls requesting that Dassault Systemes SolidWorks comes out with an eDrawings app for the iPad. So far, there have been no official announcements that this is being developed. However, this does not mean that all hope is lost. There are other Apps out there that will allow you to leverage your iPad/Android Tablet into an eDrawings wielding powerhouse. Citrix Receiver is one such App. The way it works is simple, you install eDrawings on your server at work, and then through Citrix Receiver you choose eDrawings from your “company catalog” and boom you are using eDrawings over the air on your tablet! Technology is AWESOME!!!

To learn more about Citrix Receiver you can visit the following link.
http://www.citrix.com/English/ps2/products/product.asp?contentID=1689163
eDrawings-Tablet

Reuben Felsheim

Account Manager 3DVision Technologies

Turning Parts into Assemblies, Assemblies into Parts (Part 1)

Monday, August 15th, 2011

This next series of blogs from me will be about turning Parts into Assemblies and Assemblies into Parts in SolidWokrs.

In this (Part 1) of the series, we will look at TURNING A PART INTO AN ASSEMBLY.

There are many reasons you might want to do this, the MAIN reason being something called the “Master Model” approach to modeling. Many consumer product designers do this. It is much easier to build a cell phone, or remote control, etc., as a PART file to get your form/fit/function looking good and THEN worry about “breaking up” the part into the necessary pieces to actually make the thing ! (i.e. top half, bottom half, battery door, buttons, display screen, etc.)
The great thing about this Master Model approach is then you have an ASSEMBLY (and all its individual parts) that live and breathe off of the original PART file you created. If you ever need to make form/fit/function changes you just edit the PART file and all the individual parts and the assembly would update too !!

Here’s how you do it: (there are other ways but this is the best)

Take your part file and create a SKETCH, a PLANE, or a SURFACE body that you want to use to SPLIT your part up. (can use multiple combinations of sketches, planes, and surfaces too)
Then use the INSERT–FEATURES–SPLIT command.
Select your Sketch/Plane/Surface as the “trimming tool” and hit CUT PART.
If you float around on the graphics screen you get to see what the result of the cut is going to do for you.
In the property manager under “Resulting Bodies” you will also see listed all the resulting solids that you will get from the split.
Now the important part…
If you JUST put a check mark in the box under the scissors icon, and hit OK on the command, you will just end up with a MULTI-BODY part.
If you DOUBLE CLICK in the “file name” box next to the check mark (for each body) and give it a name and location where you would like to SAVE, it will actually CREATE new parts on your hard drive representing the resultant solids !
A nice option down at the bottom of the property manager is to “Copy custom properties” from the master part to the individual parts (materials, vendor, etc.) if you would like.
Go ahead and hit OK on the command now…

In your MASTER file you DO now have a multi-body part.
BUT on your hard drive will be actual PART files from the SPLIT !
AND if you look in those part files there is a EXTERNAL REFERENCE (the “->” symbol) directly linking it back to your master model !
I.E. any changes in the master will update the parts…

Now, you could MANUALLY go make an ASSEMBLY from those individual parts, but who wants to do that !?
Look in the Feature Manager Tree of the master part. There is a SPLIT feature.
Right click on the SPLIT feature and choose CREATE ASSEMBLY.
It will go out and gather up ALL the parts that were created from the SPLIT feature and put them into an assembly with fixed relations so they won’t move ! Awesome !
(of course if you wanted to be able to move the parts in the assembly you can “float” a part and mate it into place the way you want it)

There you GO ! Turning a PART into an ASSEMBLY. WITH full associativity !

The OTHER great thing about the SPLIT feature showing up in the Feature Manager Tree of the master part is that any features you insert BEFORE the split WILL propagate down to the piece parts and to the assembly, and any thing you do AFTER the split feature will NOT.

This is a SUPER useful tool that A LOT of people can use even if you aren’t designing remote controls or cell phones. Let us know what YOU can think to use it for !

Stay tuned for Part 2 where we will show you how to turn an ASSEMBLY into a PART…

Randy Simmons

Application Engineer, CSWP 3DVision Technologies

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