Archive for the ‘Training’ Category

Borders around portions of a note in a TABLE ?

Friday, October 14th, 2011

New in SolidWorks 2010 was the ability to place a border (box, diamond, triangle, etc.) around a PORTION of a note. (we could previously only place a border around the entire note)
If you need to know how to do this, just do a search in the SolidWorks HELP file for “NOTES”, and then scroll down almost to the bottom and look for “To apply borders to entire notes or portions of notes:”

The “problem” that I want to address in this blog is the inability to do this in a TABLE.
When you are editing a cell in a General Table on a SolidWorks drawing, you only get the “Formatting” toolbar and not the property manager that you need to apply a border around a portion of the note.
So you just can’t do it, right ?

Here is the workaround…
Somewhere else on the drawing make a NOTE, and place the borders as you would like them to look in the table. While you are still editing the note, select all the text, and do a CTRL+C (copy), then to edit a cell of the table and CTRL+V (paste). There you go !!

You can of course go back and delete the note you had to make to get this. The text in the cell of the table IS editable, just don’t delete the portion with the border or you will have to do the note trick over again to get it back.

This is a LOT easier than trying to make a “custom symbol” in your symbol library…

Randy Simmons

Randy Simmons
Application Engineer, CSWP
3DVision Technologies

Turning Parts into Assemblies, Assemblies into Parts (Part 2 & 3)

Friday, September 9th, 2011

This is a series of blogs from me about turning Parts into Assemblies, and Assemblies into Parts in SolidWorks.

To see Part 1, go here: http://www.3dvision.com/wordpress/index.php/2011/08/15/turning-parts-into-assemblies-assemblies-into-parts-part-1/

This blog (Part 2 & 3) will show you TWO ways to turn an ASSEMBLY INTO A PART.

Why would you ever want to do this ?
How about if you download an assembly from the internet or your customer or colleague gives you an assembly and all you care about having is a PART file. The PART file will be smaller in file size/details and will perform better.
Perhaps you want to send your assembly to someone else but first want to “lock it down” so there will be no feature tree so they can’t change it.
Maybe you don’t want to accidentally screw up some mates in the assembly, so making it a part would accomplish this too.
I’m sure there are other great reasons…

Here is how you do it.

1st way (NON-ASSOCIATIVE):
Simple as can be, but a lot of people would never even dream of trying it…
Open your assembly, do a SAVE AS, and change the “Save As Type” drop down box to PART.
There are some options that show up then asking what exactly you would like to be saved.
Just the Exterior Faces ? The Exterior Components ? Or All Components ?
Done, easy, finished…
This method is a “one shot deal” though. It is NON-ASSOCIATIVE.
i.e. the part WON’T UPDATE if the assembly is changed.

2nd way (ASSOCIATIVE):
If you want your resulting part to actually UPDATE if you ever make changes to the Assembly it is coming from, this is the method you need to use.
The command you will use is INSERT–FEATURES–JOIN.
However, when you are in an Assembly file you can not do an INSERT–FEATURES– anything…
So the first step is to make a NEW empty part IN the assembly.
INSERT–COMPONENT–NEW PART. Select a face or plane in the assembly that you want to be the FRONT face of the new part (doesn’t really matter for what we are doing). A “side-effect” of the Insert New Part command is that it puts you into a SKETCH on that face you selected. Usually this is great, but in this case we don’t need it, so just EXIT THE SKETCH.
Now you are in EDIT PART mode in the new part, and you CAN go to INSERT–FEATURES–JOIN.
Select the parts you would like to join together into your PART file (don’t have to select them all) and hit OK.
Now if you SAVE that new part, you will have what you wanted, an ASSEMBLY TURNED INTO A PART !

In that Part file there is an external reference (the “->” symbol in the tree) showing you that any changes in the Assembly WILL propagate down to the PART.

Furthermore, if you don’t want the resulting part to be a MULTI-BODY part, you could use our boolean COMBINE command and the ADD option.

Hope you can find some uses for this !
Let us know !

Stay tuned for Part 4 !!

Randy Simmons

Randy Simmons
Application Engineer, CSWP
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

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  • 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

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  • 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

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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

Robert Warren Application Support Engineer CSWP / CSWST / CSWI / CSPS 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

Randy Simmons
Application Engineer, CSWP
3DVision Technologies

Copy Settings Wizard For Simulation? Almost.

Monday, August 1st, 2011

Have you ever wanted to copy your system settings for Simultaion? Unfortunatly the copy settings wizard just does not cut it when it comes to Simulation settings.

Here is what you need to do.

You will need to have registry permissions and knowledge of registry editor.

• Edit your registry – Select the ‘Start’ menu and then activate the ‘Run’ application. Type “regedit” and click ‘OK’.
• Navigate to- HKEY_CURRENT_USER\Software\srac\cosmos/works
• Copy Key – Right Mouse Button on the “cosmos/works” folder and select Export
• Import Key -Import the settings to a new computer. Copying this key on another machine should copy all the settings.

Simulation Key

If you’d like this option to be included in the SolidWorks copy wizard then please file an enhancement request from the SolidWorks website

Robert Warren

Robert Warren
Application Support Engineer
CSWP / CSWST / CSWI / CSPS
3DVision Technologies

“Save As” vs “Save As Copy” PART 2 (get a drawing for “free”??)

Monday, June 13th, 2011

In my last blog I discussed the IMPORTANT difference between Save As and Save As Copy in SolidWorks.

http://www.3dvision.com/wordpress/index.php/2011/06/09/save-as-vs-save-as-copy/

Now I am going to help you with what to do if you have screwed this up in the past !!

Once you understand how this works, you can FIX any references that you have messed up, AND even be able to get a Drawing of a part “FOR FREE” !

Using the FILE–OPEN window, browse to an assembly or a drawing that has incorrect references to a file.
BEFORE you hit the OPEN button, click the REFERENCES button.
You can DOUBLE CLICK on any of the referenced files, and BROWSE to a file that you would like it to reference (i.e. the correct one), OK that window, and THEN hit OPEN.
The references will be swapped !

You can also use this to get a drawing of a part for “free”.
If you have a drawing that looks like a drawing you would like to make of a different part, use the FILE–OPEN window to browse to the drawing, hit the REFERENCES button, double click the existing part file, browse to the file you want to get a drawing of, close the window, and hit the open button.
FREE DRAWING !!

Randy Simmons

Randy Simmons
Application Engineer, CSWP
3DVision Technologies

“Save As” vs. “Save As COPY”

Thursday, June 9th, 2011

I know this may be “Basic Knowledge” to a lot of you, but I still see people struggling with this and screwing up their assemblies and drawings all the time because they don’t understand it.

The only IMPORTANT thing to know about this in SolidWorks is that if you have an OPEN assembly or an OPEN drawing and you do a SAVE AS on one of the files that the assembly or drawing is referencing, it will make the assembly or drawing look at the NEW file instead of the old file !!

SAVE AS COPY will maintain the existing references, and just make a new file on the hard drive for that part.

Once you understand THAT, you will be MUCH happier in SolidWorks.

Randy Simmons

Randy Simmons
Application Engineer, CSWP
3DVision Technologies

SolidWorks Louisville User Group Meeting – June 21st, 2011

Thursday, June 2nd, 2011

2011-0601 SLUG Logo

The next SolidWorks Louisville User Group meeting – known locally as “the SLUG” – has been scheduled for Tuesday, June 21st, 2011.  It will be held at the University of Louisville Henry Vogt Engineering Center.  The meeting details are below.  If you are located in the Louisville area and have not attended a SLUG meeting, I only have one question – why not?

The topic for this meeting is “How do YOU use SolidWorks?”.  Members of the local SolidWorks Community – Scott Calvert of Design Network, Norman Boulard of Boulard Designs and Bryan Ray of  Samtec, Inc. – will be presenting some of their personal workflow and habits.  As we all know, each of us have our own way of doing things in SolidWorks.  Seeing how other individuals use SolidWorks is a great way to pick up on tips, shortcuts and learn new tools for driving SolidWorks and improving our designs.

Details

Date:  Tuesday, June 21st, 2011.  6:30pm – 8:30pm

Location:  University of Louisville, Henry Vogt Engineering Center (corner of S. 3rd St. and Eastern Parkway)

Agenda (times are approximate):
6:30pm – Registration, eat & greet
7:00pm – Meeting introduction
7:15pm – “How do YOU use SolidWorks?” presentation
8:15pm – Q & A, Next meeting discussion & prize drawings

Please RSVP to Paul McCrorey (McCrorey Digital), SLUG President, so the group leaders can plan foodstuffs accordingly.
Email:  paul.mccrorey@insightbb.com

I look forward to seeing you at the SLUG meeting!

Bill Reuss

Bill Reuss, CSWE, CSWST, CSPST
Application Support Engineer
3DVision Technologies

Mesh Control: As Easy as 1-2-3

Wednesday, April 13th, 2011

When is the last time you saw this warning dialog when meshing?  If your primary responsibilities include FEA, chances are it was as recently as yesterday.

2011-0412a Mesh Failed

As we continue to design and analyze increasingly complex models, our need to access mesh controls will increase proportionally.  Wouldn’t it be nice if accessing those tools were made simple?  Amazingly enough, they already are!  At the conclusion of a failed mesh, just click on the Mesh Failure Diagnostic button.

2011-0412b Failure diagnostics

Yes, it is that simple to access the Mesh Failure Diagnostic tools.  You’ll notice that this opens up the Simulation Advisor in the Task Pane.  The Simulation Advisor is a great tool for beginning and experienced Simulation users, alike.

Here are the 1-2-3′s of using the Simulation Advisor for applying mesh controls.
1. Select one of the parts from the list of ‘failed to mesh’ parts.
2. Click the Mesh Control button.
3. Apply the local mesh control desired to the part by either changing the slider bar or typing a value for the mesh control you wish to apply.

2011-0412d Mesh Control 123

Now click the green check mark to OK your mesh controls.  SolidWorks Simulation will mesh the component you just applied mesh control to.  Notice that you can apply mesh control to several components in one step by adding (clicking) more components to the ‘Selected Entities’ dialog box.  Another nice feature is that the Simulation Advisor window will stay open as long as you have parts that failed to mesh, allowing you to continue applying controls until your entire model has meshed.  Try using the Simulation Advisor the next time you encounter a model that is difficult to mesh!

Bill Reuss

Bill Reuss, CSWE
Application Support Engineer
3DVision Technologies

SolidProfessor for SolidWorks Users

Monday, March 28th, 2011

Did you know that SolidProfessor has products designed to help SolidWorks Users find answers to critical design questions when they need it most. . . during the design process?

SolidProfessor also delivers the most complete video library of SolidWorks instruction in the market. Included in the SolidProfessor products are Case Studies that allow you to practice using SolidWorks software and are designed to complement each step in your learning path. With these Case Studies you have access to part files, PDF guides and full video tutorials.

Right now for a limited time, 3DVision friends can access a 90 day pass to SolidProfessor 3D Skills and a 30 day access to SolidProfessor’s Modeling Tips and Techniquest archive.

Visit www.SolidProfessor.com/3dvision to register today and Keep Learning!

Carrie Cavanaugh

Carrie Patrick
Marketing Manager
3DVision Technologies