Keypad Shortcuts for Quick Views in Workbench

keypad1Hey, did you know that you can access predefined views in both ANSYS Mechanical and DesignModeler using your numeric keypad? You can! Assuming the front view is looking down the +Z-axis at the X-Y plane, here are the various views you can access via your numeric keypad.

For this to work, make sure you’ve clicked within the graphics window itself—not on the top window bar, or one of the tool bars, but right in the region where the model is displayed. You may need to turn off Num Lock, though it works for me on both my laptop and desktop with Num Lock on or off.

With that out of the way, here are the views:

0) Isometric view, a bit more zoomed in than the standard auto-fit isometric view. This is my preferred level of zoom while still being able to see the whole model, to be honest.

image

1) Front view (looking down the +Z-axis)

image

2) Bottom view (looking down the -Y-axis)

image

3) Right view (looking down the +X-axis)

image

4) Back up to the previous view

5) Isometric view, standard autofit (I don’t like the standard auto-fit—too much empty space. I prefer the keypad 0 level of zoom.)

image

6) Go forward to the next view in the cache

7) Left view (looking down the -X-axis)

image

8) Top view (looking down the +Y-axis)

image

9) Back view (looking down the -Z-axis)

image

Here’s a handy-dandy chart you can print out to refer to when using the numeric keypad to change views in Mechanical or DesignModeler. Share it with your friends.

image

A Guide to Crawling, Walking, and Running with ANSYS Structural Analysis

crawl-walk-runAt PADT, we apply a Crawl, Walk, Run philosophy to just about everything we do. Start with the basics, build knowledge and capability on that, and then continue to develop your skills throughout your career. Unfortunately, all too often I run across some poor new grad, two weeks out of school, contending with a problem that’s more befitting someone with about a decade of experience under his or her belt.

Now, the point of this article isn’t to call anyone out. Rather, I sincerely hope that managers and supervisors see this and use it as a guideline in assigning tasks to their direct reports. Note that the recommendations are relative and general. Some people may be quite competent in the “run” categories after just a few months of usage and study while others may have been using the software for a decade and still have trouble figuring out how to even start it. It’s also possible that, for certain projects, the “crawl” categories may actually end up being more difficult to contend with than the “run” categories.

With those caveats in mind, here is our list of recommendations for Crawling, Walking, and Running with ANSYS. Note that these apply to structural analysis. I fully plan to hit up my colleagues for similar blog posts about heat transfer, CFD, and electrical simulation.

Crawlsimple-stress1

  • Linear static
  • Basic modal
  • Eigenvalue (linear) buckling, but don’t forget to apply a knock-down factor

Walkstruct-techtip6-contacts-between-bolts

  • Nonlinearities
    • Large Deflection
    • Rate-independent plasticity
    • Nonlinear contact (frictionless and frictional)
  • Dynamics
    • Modal with linear perturbation
    • Spectrum analyses (running the analysis is easy; understanding what you’re doing and interpreting results correctly is hard)
      • Shock/Single point response
      • Random Vibration (PSD)
    • Harmonic analysis
  • Fatigue

Runvibration-pumping platforms

  • Nonlinearities
    • Advanced element options
    • Hyperelasticity
    • Rate-dependent phenomena
      • Creep
      • Viscoelasticity
      • Viscoplasticity
    • Other advanced material models such as shape memory alloy and gaskets
    • Element birth and death
  • Dynamics
    • Transient dynamics (implicit)
    • Explicit dynamics (e.g. LS-Dyna and Autodyn)
    • Rotordynamics
  • Fracture and crack growth

So what’s the best, quickest way to move from crawling to walking or walking to running? Invest in general or consultative (or even better, both) ANSYS training with PADT. We’ll help you get to where you need to be.

Peeling Away the *VMASK

vmask-icon2One way to really unleash the power of APDL is to become familiar, and ultimately fluent, with array parameters. The APDL student will quickly learn that array manipulation involves heavy use of the *V commands, which are used to operate on vectors (single columns of an array). These commands can be used to add two vectors together, find the standard deviation of a column of data, and so on. *V commands consist of what I like to refer to as “action” commands and “setting” commands. The action commands, such as *VOPER, *VFILL, and *VFUN * have their own default behaviors, but these defaults may be overridden by a preceding setting command, such as *VABS, *VLEN, or *VMASK.

*VMASK is one of the most useful, but one of the most difficult to understand, *V command. At its essence it is a setting command that directs the following action command to a “masking” array of true/false values. Only cells corresponding to “true” values in the masking array are considered for the array being operated on in the subsequent action command.

For example, a frequently used application of *VMASK is in the compression of an array—for instance to only include data for selected entities. The array to be compressed would consist of data for all entities, such as element numbers, x-locations for all nodes, etc. The masking array would consist of values indicating the select status for the entities of interest: 1 for selected, –1 for unselected, and 0 for not even in the model to begin with. Only array cells corresponding to a masking array value of 1 would be included in the compression operation, with those corresponding to a value or 0 or –1 being thrown out. Here is a slide from our APDL training class that I hope illustrates things a little better.

image

Take the class or buy the manual (and review it at Amazon, please!)

What we’ve learned so far is that the masking array contains a list of true/false (or not true) values to refer to when performing its vector operation. But actually, it’s much more general than 1, 0, and –1. What *VMASK does is include cells corresponding to all positive numbers in the masking array (not just +1) and exclude cells corresponding to all values less than or equal to zero in the masking array (not just 0 and            -1), which broadens the possibilities for how *VMASK can be handy.

Everything I’ve used *VMASK for up to this point in my career has involved array compression, and I figured I’d be put out on a sweep meshed ice floe into a sea of CFD velocity streamlines (that’s what happens to old CAE engineers; you didn’t know that?) before I came up with anything else. However, I recently ran into a situation where I needed to add up just the positive numbers in an array. I was about to construct an algorithm that would test each individual number in the array to see if it was positive and, if so, add it to the total. It would’ve been cumbersome. Then I came up with a much less cumbersome approach: use the array as it’s own masking array and then perform the addition operation. Let’s look at an example.

Take the following array:

image

The sum of all values in the array is 1.5 whereas the sum of just the positive values is 11.5. What’s the most efficient way to have APDL calculate each?

In the case of summing all values in the array, it’s easy, just simply execute

*VSCFUN,sum_total,SUM,sum_exmpl(1)

which gives you

image

But what about summing just the positive values? That’s easy, just use SUM_EXMPL as its own masking array so that only the positive values are included in the operation.

*VMASK,sum_exmpl(1)

*VSCFUN,sum_pos,SUM,sum_exmpl(1)

image

Boo yeah

Now why was I doing this? I had to create a macro to calculate total nodal loads for an unconstrained component in just the positive direction (to ignore the loads counteracting in the negative direction), and this was my approach. Feel free to download the macro: facelds.mac and try it out yourself.

Vibro-Acoustics Analysis in ANSYS Mechanical as Told by a Structures Guy

Vibro-Acoustics-ANSYS-iconWith the introduction of ACT, the ANSYS Workbench editors have gained capabilities and shortcuts at much faster rate than what can be introduced in a development cycle. One of first and most far-reaching extensions is the acoustics. Inevitably I was called on by one of our customers to show them how to do a vibro-acoustics analysis (harmonic with acoustic excitation), which I did. Since the need for this type of analysis is quite broad, I’ll share it here too.

There was an extra level of excitement with this, in that I’m a structures specialist with no prior acoustics experience. So, I did my own self-training on this topic. I have to give tons of credit to Sheldon Imaoka of ANSYS Inc., who took the time to thoroughly answer the questions I had. That being said, this article will be from the standpoint of a structures engineer who’s just recently learned acoustics.

The first thing you’ll need to do is download the Acoustics extension from the Downloads section at the ANSYS Customer Portal and install it in Workbench.

image

It’s at the very top, under ‘A’ for “Acoustics”

One thing you’ll notice when you unzip the Acoustics Extension package is that it contains and entire Acoustics training course. Take advantage of this freebie when learning acoustics analysis. I’ll note that, most of the process outlined in this article comes from the Submarine workshop in the acoustics training course.

Once you’ve installed and turned on the Acoustics extension, insert a Harmonic Analysis system into the project schematic, link to the solid geometry file, and specify the material properties for the solid. You’ll specify the properties for the acoustic region in Mechanical under the appropriate Acoustics extension objects.

image

Rename as you see fit

Assuming you just have the geometry for the solid and not the acoustics domain, create two acoustics regions around the solid. The first region, surrounding the solid, will function as the fluid region itself, through which the acoustic waves travel and interact with the structure. The second region, surrounding the first acoustics region, will function as the Perfectly Matched Layer (PML). The PML essentially acts as the infinite boundary of the system. (If you’re an electromagnetics expert, you already know this and I’m boring you.) You can easily create these domains using the enclosure tool in DesignModeler.

image

Acoustics Regions

Now we’re ready for the analysis. Open up Mechanical. Look at all those buttons on the Acoustics toolbar! Yikes! Fortunately we just need a few of them.

image

Here they are

Insert an Acoustic Body and scope it to the acoustic region surrounding the structural solid. In the Details, enter the density and speed of sound for the fluid. Also set the Acoustic-Structural Coupled Body Options to Coupled With Symmetric Algorithm.

image

image

image

Pay attention to the menu picks, Details, and geometry scoping here and in the rest of the image captures

“Coupled” refers to coupled-field behavior, i.e. the mutual interaction between the structure and the fluid. You’re probably familiar with this. You need that, otherwise the acoustic waves are just bouncing off the structure and the structure isn’t doing anything. Regarding the Symmetric Algorithm: The degrees of freedom for the acoustic system consists of both structural displacements and fluid pressures, giving you an asymmetric stiffness matrix. However, ANSYS has incorporated a symmetrization algorithm to convert the asymmetric stiffness matrix to a symmetric matrix, resulting in half as many equations that need to be solved and thus a faster solution time yadda yadda yadda, so go with that.

Now insert another Acoustic Body, this time scoped to the outer acoustic region (body). This is your Perfectly Matched Layer. Specify fluid density and speed of sound as before. This time, leave the Coupled Body Option as Uncoupled. But, set Perfectly Matched Layers to On.

 imageimage

Apply an Acoustic Pressure of zero to the outer faces of the PML body (Boundary Conditions > Acoustic Pressure). As you may have guessed from the menu pick, this is your acoustics boundary condition.

clip_image020imageimage

Now we’ll apply some acoustic wave excitation to this thing. From the Excitation menu, select Wave Sources (Harmonic). In the Details, set the Excitation Type to either Pressure or Velocity, set the Source Location and specify the excitation pressure or velocity value. In this example, I went with Pressure since that’s what MIL-STD-810 specifies, but this option will be based on your customer requirements. I also assumed an external acoustic source (hence, Outside the Model), but again, that will be based on your particular project. You also need to specify the vector of the wave source, via rotations about the Z and Y axes (f and q). In this case I chose 30 and 60 degrees, respectfully, to make it interesting. Once again, enter the density and speed of sound for the fluid.

clip_image026image

Insert Scattering Controls under the Analysis Settings menu and specify whether the Field Output should be Total or Scattered. Total gives you constant pressure waves that interact with the solid but not each other. Scattered gives you wave that interact and interfere with each other as well as the solid.

imageimage

Set up the Fluid-Structural Interaction boundary condition where the structural faces are “wetted” by the acoustic domain. The FSI Interface is found under the Boundary Conditions menu.

imageimage

Apply structural constraints and specify harmonic analysis settings just like you would with a standard harmonic analysis. Make sure you request Stresses under the Output Controls. Solve the model.

imageimage

Plot your structural results as you would for a typical harmonic analysis. Acoustic Pressure wave results may be found under the Results menu in the Acoustics toolbar. If you used Total field output for the scattering option, you can verify your wave source direction by looking at the Acoustic Pressure Contours. Keep in mind that the contours will be orthogonal to the axis of the sine wave; you may need to put some extra spatial thought into it to fully understand what’s going on.

imageimage

image

Acoustic Pressures: Field Output = Total

image

Acoustic Pressures: Field Output = Scattered

image

Von-Mises Stresses, Max Over Phase: Field Output = Scattered

As you’ll note in the training course, there are a number of design questions that can be answered with acoustics analysis. In this article, I’ve addressed what I thought would be one of the more popular applications of acoustics simulation. If the demand is there, I’ll research and compose more articles on various acoustics applications in the future. For instance, another area I’ve examined is natural frequencies of a structure that’s submerged in a fluid. If there’s another acoustics topic you’d like us to write about, please let us know in the comments.

IGES Can’t Stand IGES Anymore!

Users:

I got some errors when I imported my geometry.
I have some holes and stray surfaces in my geometry.
The edges are twisting around on my geometry import.
ANSYS blows up when I’m trying to mesh my imported geometry.

Me:

What geometry format are you using?

Users:

IGES.

IGEEEEEEESSSSSS!!!

The vast majority of the time, geometry import errors are attributable to the choice of geometry format. And that choice is IGES. To understand the problems with IGES, it helps to know a little bit of IGES history.

IGES, which stands for Initial Graphics Exchange Specification, was released in 1980 as a neutral format for sharing data between CAD systems. The most recent version, 5.3 came out in 1996.

2009_09_21_izzy

IGES: The “Izzy” of geometry formats

Besides being old, there are a few other problems with this format:

  • IGES only contains surface information. When the IGES file is read in, ANSYS has to take the additional step of creating a volume from the region enclosed by the surfaces. The IGES file contains no additional information about how the surfaces should be stitched together, so ANSYS has to figure it out, leading to possible errors, particularly with assemblies.
  • Each CAD application has its own tolerances when exporting to IGES, and loose tolerances are more likely to lead to errors in the ANSYS import.
  • Somewhat related to the previous bullet point, IGES is a middleman between the CAD system and ANSYS, creating two paths for error propagation: Exporting from CAD to the IGES file and importing the IGES file into ANSYS.

Generally speaking, IGES is typically the worst geometry format to import into ANSYS.

Now that I’ve trashed IGES, here is what I recommend:

Native Geometry

ANSYS offers several native geometry readers, such as Connections for Pro/E, NX, Solidworks, SolidEdge, etc. that bring in geometry directly from the CAD modeler. There are two advantages here:

  1. Geometry comes over directly from the CAD tool, therefore no tolerance errors propagating through a neutral geometry format “middleman.”
  2. CAD readers allow for bi-direction associativity between the CAD tool and Workbench, so a Workbench model can be refreshed to reflect updated geometry which still retaining mesh settings, loads, etc. Also, the CAD model can be refreshed based on updated geometry in Workbench.

The only catch when it comes to native geometry readers is that they require a separate license. However, about 90% of the tech support calls I’ve received about IGES import errors are from people who have licenses for native geometry readers and just aren’t using them.

Even if you have a native geometry reader license, you’ll need to be sure to check the box to install the reader during ANSYS installation. You may also need to use the CAD Configuration Manager (found in the Utilities folder in the ANSYS start menu) to configure the CAD reader if you didn’t do so during installation.

The one unfortunate exception to this is CATIA. The CATIA kernel is a bit more guarded than the other CAD kernels, and this is frequently noted in CATIA geometry import errors. Also, you can only import CATIA geometry, not associate to it as with other CAD tools.

Neutral Files That Aren’t IGES

Your ANSYS installation comes with the capabilities to import both IGES and STEP files without having to purchase an additional geometry connection license. Of the two, STEP is typically the better option. There are two reasons for this:

  1. STEP (which stands for “Standard for the Exchange of Product model data,” because these people do not bow down to society’s piddly  rules of acronym construction) contains true 3D volume definitions, instead of having to construct volumes between enclosed surface regions post-import, so the solid model definition ends up being more robust.
  2. STEP was first developed in 1984 and continues to be developed, even as recently as 2011, so export/import errors are regularly addressed, unlike with IGES.

You may also have licenses for Parasolid and/or ACIS readers, which can lead to some confusion as to which format to use. This is easily addressed by considering the underlying geometry kernel for the originating CAD tool*.

I said geometry kernel, not…oh never mind… mmmm… fried chicken….

For example, SolidEdge, NX, and Solidworks all use the Parasolid kernel. Therefore the most robust neutral format for geometry exported from these tools will generally be Parasolid (.x_t or .x_b extension), of course. Likewise, AutoCAD uses the ACIS kernel, indicating that ACIS (.sat file) will usually be the best neutral geometry format in this case. For CAD tools that use neither of these kernels, STEP will typically be the best neutral format.

As you can see, even though the IGES people know how to make acronyms, IGES is typically the last geometry format you want to try when importing or associating geometry to ANSYS. This doesn’t mean that IGES is always the worst option for reading in CAD files (especially compared to the CATIA connection), just that it usually is.

*Hat tip to Robin Steed of ANSYS, Inc. for this tip

Be a View Master: Customizing and Managing Views in ANSYS Mechanical

Accessing various predefined views in Mechanical is easy. You can click on the triad axes (including the negative sides of the axes) and view the model down those axes, or click the turquoise isometric ball for an isometric view. Or you can right click the graphics area and select from a variety of views (top, back, left, etc.) from the View menu.

But what if you want a predefined view that has the model rotated “just so” and zoomed out “just so?” What if you want to store these settings not just in your current model, but bring them into other models as well? Starting in R14.5 you can do this, using the Manage Views window.

To open the Manage Views window, click on the eye-in-a-box icon that looks like it was designed by Freemasons. image The Managed Views window appears at the lower left of the GUI. The window consists of the following:image

The labels are pretty self-explanatory, but let’s delve into a couple of examples. As you can see by observing the triad, the model viewpoint shown here does not coincide with any pre-defined view.

image

Click the Create a View button image and give the view a name (defaults to View 1 but any name can be given):

image

After rotating, panning, and zooming, you can return to this view by clicking the Apply a View button. image

image

As mentioned before, you can apply the same view between different models by using the View Export/Import capabilities. To do this, simply highlight the named view to be exported in the originating model and click the Export button. image Specify the xml file to which the view is to be stored. In another model, click the Import button image and browse to the xml file containing the view to be imported. This is basically the Mechanical equivalent of an APDL file containing /VIEW and /ZOOM commands. Example follows.

The following view is to be stored and exported to another model. Highlight the view name (“Sulk”) and click the Export button.

image

Frankie the Frowning Finite Element Model worries that views can’t be shared between models.

Specify the xml file name and click Save.

image

In a different model, click the Import button, browse to the xml stored in the previous step, and click open.

image

Highlight the imported view name and click the Apply a View button.

image

Sammy the Smiling Simulation Model is happy that views can be transferred between models.

The Managed Views window provides a significant amount of viewing versatility over the standard viewing definitions.

Efficient Engineering Data, Part 2: Setting Default Materials and Assignments aka No, You’re Not Stuck with Structural Steel for the Rest of Your Life

Longer ago than I care to admit, I wrote an article about creating and using your own material libraries in Workbench. This is the long awaited follow-up, which concerns setting the default Engineering Data materials and default material assignments in Mechanical and other analysis editors.

imageNote:
Part of the reason it’s taken me this long is that I moved to New Mexico to help staff PADT’s new office there, and to shadow Walter White. It has been a hectic, exhausting endeavor but I’m here and I’m finally settled in. If you’re in New Mexico and are interested in ANSYS, engineering services, product development, or rapid prototyping (e.g. 3D printing), please feel free to contact me.

In order to make the best use of the procedures here, you will probably want to know how to create your own material libraries. Part 1 describes how to do this. This will also work with the material libraries that come with the ANSYS installation, though.

Pick Favorites

The first step is to get into Engineering Data and expose the material libraries by clicking on the book stack button ( image ). Then, drag the materials of your choice from the appropriate library(ies) to the Favorites Data Source. These can include materials you want to have available in Mechanical by default as well as materials that you would like to consolidate into a single location for quick access. At this point, the default material availability and assignments have not been altered. These will be handled in the next couple of steps.

image

Drag and Drop Materials to Favorites

Set Default Material Availability

To specify which materials will be immediately available for assignment in future analyses, go to the Favorites Data Source and check all applicable materials in column D. Though not assigned to the immediate set of engineering data, these will be on the default list of available materials in subsequent analyses, i.e. when you create a new analysis in the same project schematic or when you exit and reopen Workbench.

image

Check to Add to Default List of Available Materials

image

Materials Immediately Available Inside Mechanical

Set Default Material Assignment

Now our most commonly used materials are immediately available in our analysis editor. But Structural Steel still lingers. In many, if not most, cases, we would prefer our default assignment to be something else.

The fix is easy. Once again, go to the Favorites Data Source, right click the material you wish to have as your default material, and select Default Solid Material (and if you’re doing Emag or CFD, you can set your default fluid or field material with the right-click menu too). Your default solid material will now replace Structural Steel in subsequent analyses.

image

Example: Aluminum 6061-T651 Set as Default Material Assignment

image

Becomes Default Material Assignment in Analysis

Note that you can stop at any step in this process. If you want to consolidate favorite materials, but don’t want to have them immediately in your analysis editor, you can do that. If you want a default list of materials to select from without specifying a default material assignment, you can do that too. More than likely, though, you’ll want to do all three.

Efficient Engineering Data, Part 1: Creating and Importing Material Properties in Workbench

Note: This is part 1 of a two-part series in Engineering Data customization and default settings. This article essentially serves as a foundation for my next one, which will cover how to set up default material choices and assignments in Workbench.

As you’ve probably noticed, the Workbench installation comes with an extensive set of material libraries. If you haven’t noticed, then open a Workbench session, go into Engineering Data, and click that button on the upper right that looks like a stack of books: image

Click on one of the libraries, say, General Materials, and take a look at the selection of materials.

image

So you see things like Stainless Steel, Aluminum Alloy, Titanium Alloy, etc. but which alloys exactly? 301 1/2-hard steel? 17-4PH? 6061-T6 aluminum? Or cast C355? Titanium 6-4? Or 6-2-4-2? Obviously you’re going to have your own material properties in mind, and you’ll probably use them frequently enough to where you’d like to have them readily accessible. Maybe store them in a library, or something.

As it turns out, you’re not confined to the libraries ANSYS provides with the Workbench installation. You can create your own libraries too. To start this off, first click in the first blank line in the top Engineering Data Sources section, where it says, “Click here to add a new library” (seems pretty straight-forward, doesn’t it?) and type a unique name for the library. I’ll call mine “Jeff’s Materials” because I’m incredibly original that way. Then hit Enter.

image

image

You’ll be prompted for a location and xml file name for the library. Specify these and click Save. All of your material names and properties will be stored in this file.

image

Notice that the new library is checked. That means it is unlocked and able to be edited.

image

At that point you can add material names, insert properties from the left side Toolbox, etc.

image

Type in some material names

image

Then define their properties

Once you’re finished adding and editing materials, uncheck the column B box of the library to lock it up. Click Yes to accept changes. If you want to add or edit materials to your library at a later date, simply unlock it by checking the column B check box again.

image

Now, let’s say you want to share your awesome material library with your co-workers, or maybe you’ve installed a new version of ANSYS and you want to include it, or maybe your library was deleted by gnomes during the night. How do you bring it back into Workbench? Simple. First make sure the xml file is available (you’ll want to email it to your co-workers and have them save it to their disks if you’re sharing it with them). Toggle the libraries on by clicking on the stack of books button. Then simply click the little ellipsis button on the “Click here to add a new library” line.

image

Browse to the appropriate xml file and open it.

image

And now you have your library back.

image

I was too lazy to define all the materials for this article, hence the question marks

This is all well and good, but wouldn’t it be nice if we could change the materials that are immediately available in Engineering Data upon opening Workbench, and set the default material assignment to something besides Structural Steel? As it turns out, you can do both of these, and I’ll show you how in the next installment of Efficient Engineering Data.

Visualizing Nodal Connectors in Mechanical

As I noted in my series on nodal interactions in Mechanical, ANSYS has been exposing more capabilities to interact with the underlying finite element model over the past couple of versions. Additionally, Mechanical’s visual verification capabilities have improved as well, as it is now possible to view nodal connectors created by remote forces and displacements, weak springs, and MPC contact.

To demonstrate this, I’ve modeled a ball valve as shown below.

image

The model is set up with the following options and boundary conditions. (Don’t try to make real-life sense of these; I’m just demonstrating capabilities here.)

  • Weak springs are turned On under Analysis Settings.
  • The bonded contact between the handle and shaft is set to MPC behavior (the bonded contact between between the valve body and ball is kept as Program Controlled).
  • A 50 lb remote load is applied just off the end of the handle and scoped to the end face of the handle (B in the figure above).
  • A 5 degree Z-rotation is applied as a remote displacement and scoped to the front face of the valve body (C in the figure above).

Now, you won’t be able to view the “spider webs,” “bicycle spokes,” etc. generated by the nodal connections yet. The weak springs, MPCs, and beams are not created until the matrices are assembled. So, at this point you will want to solve the model.

When the solution is complete, highlight the Solution Information folder in the Model tree. You will see two tabs at the bottom of the graphics window: Graphics and Worksheet. Click on the Graphics tab.

image

You will now see all the nodal connections displayed for your finite element edification, and they are glorious. Note: Constraint equations (CEs) include multi-points constraints (MPCs).

image

Click the Show Mesh button for the full finite element display.

image

The “clumping” of the MPCs on the front face of the valve body might look a little odd, and it is—you’re not imagining it—but it deflects the way I expect it to, so I’m good with it.

Now right about now, you’re yelling at me through your monitor and I can hear what you’re saying. “Hey, Strain, I don’t have the luxury of working with these little Mickey Mouse sample models that you create for sales demos or training courses or Focus articles! The models I make are real-life models that take hours or days to solve. Do you really expect me to wait for hours or days before I can verify that my connectors are correct?” Fret not, dear ANSYS user; there is a simple workaround to this. When the Solution Status says “Solving the mathematical model,” simply click [Stop Solution] and continue to display the connectors as described above. Maybe give it a minute or two first, though, just to make sure the matrices have been assembled and the connectors generated.

image

The default is that you see everything, displayed as lines, but if you take a look at the Solution Information details, you’ll see that you have some additional display options under FE Connection Visibility.

image

By default, we see All FE Connectors, but we can switch the Display option to CE Based, Beam Based, or Weak Springs. (We can also change it to None, but that would defeat the purpose of this article.) Here is the same model with Display set to Weak Springs.

image

image

By default, the connections for all nodes are displayed, but you can isolate the display to a nodal named selection under the Draw Connections Attached To option. For example, here is the connector display for the front valve body face nodes, named “front face nodes.” (Note: I’ve turned all FE connectors back on.)

image

image

Finally, if you want a bit more visual clarity, you can change the Display Type to Points instead of Lines.

image

image

This is another example of direct finite element interaction being enabled in Mechanical. With this capability, the user will no longer need to export the model to Mechanical APDL for visual node connector verification. Expect even further finite element interaction capability in future versions; ANSYS is on a roll in this area.

Composite Sketching, ANSYS Style: Copying a Sketch from One DesignModeler Session to Another

Recently a customer approached me and told me that he had a sketch in one DesignModeler database that needed to be copied over to another DesignModeler database and asked me if it would be possible to do so. My initial reaction was, “No way, dude be trippin’,” because that’s how I talk in professional settings. But, I really wasn’t ready to assert its impossibility without first digging into it a bit, so that’s what I did.

Clicking around the DesignModeler menus (Ever wonder how we ANSYS support professionals figure things out? Now you know.) I found something that had flown under my radar previously. Under the File menu are a couple of selections indicating the ability to write and read sketch scripts. Pay dirt.

So, what is it that these wonderful scripts can do for us? Let’s take a look. Say, for example, you have two separate sketches in two separate DesignModeler sessions. I have labeled these sessions “Face” and “Head.” See if you can figure out which is which.

imageimage

(Side note: It may be hard to believe, but this is not the original geometry the customer was working with)

Now, keeping in mind that these are two completely different DesignModeler databases, how can I copy the Face sketch, including dimensions, and paste it on top of the Head sketch? The answer is simple. First highlight the DesignModeler plane containing the Face sketch.

image

Next, click File > Write Script: Sketch(es) of Active Plane. You will be prompted for a file name and location of the resulting jScript file. Specify those and click [Save].

imageimage

Note that all of the sketches on the selected plane will be written to the jScript file. If there are any sketches you don’t want to keep, you can always delete them later.

Next, move over to the Head model. Highlight the plane you would like to copy the Face sketch to. In this case, it is the XYPlane again, but you can pick whatever plane you want; it doesn’t have to be the same plane between sessions. The sketch will maintain its position relative to the origin of whichever plane you select.

image

Next click File > Run Script and select the jScript file that was written previously. Click [Open].

image

image

More than likely, you will get a warning about modifying the feature number to avoid duplicates. This is normal. It simply means that it’s renumbering the imported sketch to avoid having, for example, two “Sketch1” objects. Click [OK].

You will now see the Face sketch, dimensions and all, overlaid on the Head sketch. The Sketch object has been renumbered and placed onto the XYPlane.

imageimage

And, as you can see, everyone is happy.

Node Interaction in Mechanical, Part 4: Scoping Results to Nodes

This article is the eagerly awaited fourth and final installment in my series on interacting with nodes in ANSYS Mechanical. To review, the previous three articles covered picking your nodes, creating named selections from nodes, and applying boundary conditions to nodes.  I know some of you were wondering why it took a while for this final article to come out. Well, I’d been sent to my home state of Indiana for business and decided to take a few extra days to visit relatives—living and not-so-living.

photo

Great-great-great-great-great grandpa!

Now on to business. Our discussions so far have centered on preprocessing and solution processing operations with nodes. Now we’ll conclude the series by covering postprocessing operations with nodes in Mechanical. Much the same way that you can scope boundary conditions to nodes, you can also scope results to nodes. There is one key difference however: whereas nodal boundary conditions can only be scoped to named selections, nodal results can be scope to geometry or named selections.

Scoping results to nodes based on geometry selection is accomplished using the same procedure as scoping results to any other geometry: simply select the nodes of interest, and insert results.

image

image

Likewise, for named selections, simply insert the results object of interest, set the Scoping Method to Named Selection and choose the appropriate named selection.

image

image

Does something appear a bit unusual about that last figure? Notice that the results are plotted as continuous contours, with the nodes emphasized, rather than just appearing as discrete points. When all of the nodes on an element are selected, such as in this example, the results are displayed as a continuous contour across the face. Here’s an example showing what happens when some element faces have all their nodes selected, and others have only a few.

image

image

Beyond the standard analysis results, you can perform some additional nodal orientation verification as well. Remember how in the third article in this series I sent the Mechanical modal over to Mechanical APDL and turned on the nodal coordinate systems there to verify their orientations? Now you do, because I linked you to it. Well, as it turns out, you can get the same information in Mechanical. Let’s see how.

As an example we’ll start with the same valve with a cylindrical coordinate coordinate system located at the center of the outlet flange. The nodes on the outlet flange face (Named Selection: Outlet Flange Nodes) have been rotated into this cylindrical coordinate system and a 0.01” displacement applied to them in the Y (theta) direction. The inlet flange is fixed.

image

After solving the model, highlight the Solution branch and click on the Coordinate Systems pulldown, way on over to the right of the Solution toolbar, next to the Command Snippet button.

image

Using this pulldown menu, you can display nodal coordinate triads and nodal rotation angles. The Nodal Triads pick displays the nodal coordinate systems, equivalent to executing /PSYMB,NDIR,1 in Mechanical APDL.

image

The Nodal Euler Angles display the amount of nodal rotation in each plane from the original position. Here’s a plot of the Nodal Euler XY Angles of the outlet flange nodes.

image

Wait a second. Don’t those contours seem a little “off” to you? They’re not lined up radially, and the zero and 180 degree rotation values aren’t quite located where I expect them to be. Wait, I think I know what the problem is. Let’s set the displacement scaling to 0.0 (Undeformed) and see what happens.

image

There, that’s better.

Note that you can also display element triads and Euler angles, for rotated element coordinate systems, but that’s a topic for another day.

This completes the nodal interaction series for R14.0 ANSYS Mechanical. We will be sure to keep you informed of further improvements to finite element interaction capabilities in Mechanical as future versions are released.

Node Interaction in Mechanical, Part 3: Nodal Boundary Conditions

This article is Part three in a four-part series about taking advantage of the new nodal interaction capabilities in Workbench 14.0. In Part 1 I discussed how to pick nodes and retrieve information about them. In Part 2 I covered various methods of creating nodal Named Selections. In this installment I’ll address the procedures for applying loads and constraints to mesh nodes, as well as rotating them into different coordinate systems.

All of the nodal boundary conditions, including nodal rotations (which I realize isn’t a boundary condition, per se, but it does affect how boundary conditions are applied) may be found in the Direct FE pull-down menu when the Analysis branch is highlighted.

imageimage

One key thing to note about all of the nodal boundary conditions is that they may only be scoped to Named Selections, not Geometry Selection. So before you continue, make sure you’re well versed in nodal Named Selection creation.

Stepping through the Direct FE commands in menu order, the first item we come to is Nodal Orientation. This is how we rotate a node to another coordinate system. Of course, to be able to reorient a node to another coordinate system, we will have to create one first. Once that’s done, select Nodal Orientation from the Direct FE pull-down menu.

In this case, we will rotate the nodes belonging to the named selection EndNodes to a cylindrical coordinate system I created at the end of the tube called Cylindrical Coordinate System (because I’m original like that).

imageimage

Click Direct FE > Nodal Orientation. In the Details window set the Named Selection to EndNodes and Coordinate System to Cylindrical Coordinate System. Easy peasy. Note that the Scoping Method cell is grayed in with “Named Selection,” indicating that you can’t change it.

image

Just as in Mechanical APDL, all forces and constraints are applied in the nodal coordinate system, defined by the Nodal Orientation. In this example, I applied FE Displacement constraints in the X (radial) direction and Nodal Forces in the Y (theta) direction and verified them in Mechanical APDL.

image

One thing to keep in mind is that Nodal Orientation is rarely necessary, since loads and constraints applied to solid model entities may be applied in user defined coordinate systems and Frictionless Supports rotate nodes to be normal to the surface.

Moving along, for the Nodal Force example we will apply a downward force to the 12 nodes contained in the Named Selection EndFaceNodes.

image

Following a similar procedure as before, click Direct FE > Nodal Forces. Set the Named Selection to EndFaceNodes and enter –1200 lbf for the Y Component of force. Note that Nodal Coordinate System is set in gray for the Coordinate System selection. The key item to note, however, is the Divide Load by Nodes option. If set to Yes, the load will be split evenly between the nodes, in this case 1200 lbf/12 or 100 lbf per node, for a total of 1200 lbf applied. If set to No, the full load is applied to each node in the Named Selection, giving a total applied load of 1200 lbf x 12 = 14,400 lbf total.

image

Here are the Probes of the Reaction Loads with the Divide Load by Nodes option set to Yes and No.

Divide Load by Nodes = Yes

image

Divide Load by Nodes = No

image

To applied pressures to nodes, click Direct FE > Nodal Pressure and specify the Named Selection and pressure value. Note that the pressure can only be applied in the normal direction to nodes. Also note that, at a minimum, the nodal Named Selection has to consist of all the corners on an element face for the pressure to have any meaning.

image

image

Apply constraints directly to nodes by clicking Direct FE > FE Displacement. Specify the Named Selection and enter the displacement values in the nodal coordinate system X, Y, and Z direction (or leave Free).

image

Nodal rotations (Direct FE > FE Rotation) may only be applied to nodes attached to elements with rotational degrees of freedom, such as beams and shells. The rotations themselves can only be fixed (i.e. zero degrees) or free. At this time there is no capability to impose a finite nodal rotation.

imageimage

In the next and final installment, I will discuss how to scope results to nodes and verify nodal and element orientations. Get ready to be thrilled.

Node Interaction in Mechanical, Part 2: Nodal Named Selections

This is the second entry in a thrilling saga about interacting with nodes in ANSYS Mechanical. In Part 1, I addressed the various methods for picking and querying nodes in a Mechanical model. In this entry, I discuss various methods for creating nodal Named Selections. Creating nodal Named Selections is a key step in executing the processes I’ll address in my next two entries: Applying nodal boundary conditions and scoping results to nodes.

I’ll start with the easy stuff. To create a Named Selection from picked nodes, simply pick the nodes you’re interested in as described in Part 1, right-click, and select Create Named Selection (or, in the Named Selection toolbar, click the Create Named Selection) and give it a name.

image

Note that the “Apply geometry items of same:” option does not work with nodes yet. However, there is another option: The Worksheet. The worksheet will allow you to define nodes based on location, node number, and attachment to solid model entities.

To activate the Worksheet mode, highlight the Named Selection branch (add it from the Model toolbar if necessary) and insert a new Named Selection. In the details window, change the Scoping Method from Geometry Selection to Worksheet.

image

The Selection worksheet appears.

image

To begin the selection process, right click on the first row and select Add Row.

image

image

The Add action is similar to selecting “from full” or “also select” in Mechanical APDL and is most likely the first action you will take in the selection process. Select Mesh Node from the pull-down menu under Entity Type.

image

For the criterion, select either Location X, Y, or Z or Node ID (node number).

image

Then select the appropriate Operator from the pull-down menu. Available options for both Location and Node ID are Equal, Not Equal, Less Than, Less Than or Equal, Greater Than, Greater Than or Equal, and Range. Options for Location additionally include Smallest and Largest.

image

Next, fill in the Value, Lower Bound, and/or Upper bound as appropriate. Also select the appropriate coordinate system when using one of the Location criteria.

image

When complete, click the Generate button to execute. The Geometry entry in the details will indicate the number of selected nodes. Click on the Graphics tab to verify the selection.

image

image

If desired, add additional selection actions. The Add action at this point behaves as “also select.” Remove behaves as “unselect.” Filter acts as a “reselect” operation. In this example, we will Filter the selection to nodes between Y = 0 and Y = 2.5 inches. (I also could’ve simply done Y > 0, but I wanted to show the Range Operator here.)

image

image

At this point, you’ve probably noticed that the Named Selection is named “Selection.” Simply rename it by right clicking on the Selection object and selecting Rename.

So now you know how to create nodal Named Selections based on location and node number, but how do you create a named selection from nodes attached to a face or some other solid model entity. That’s a little more complicated, but I’m here to take you through it. It’s not really difficult once you know the steps.

First, create a Named Selection from the geometric entities containing the nodes you want to select.

image

Then create a new Named Selection with the Worksheet scoping method. In the first row set Add as the Action. Set the entity type equal to the entity type the Named Selection was created from in the previous step. Set the Criterion to Named Selection and the Operator to Equal. Select the Named Selection created in the previous step from the pull-down menu under Value.

image

“Criminy, Strain! We’re just selecting the same Named Selection that we create in the previous step! What’s the point?! You’re wasting my time!” Read on; there’s another step here.

Add another row to the Worksheet. Set the Action to Convert to and the Entity Type to Mesh Node. Then click Generate and verify the selection in the graphics window. There, don’t you feel silly for getting so upset in the previous paragraph?

image

image

In these first couple of parts, we’ve spent a lot of time learning how to simply select the nodes. Now wouldn’t it be nice to actually do something with them? In the next two parts, we’ll do exactly that. First, we’ll see how to apply loads and constraints directly to nodes, and rotate them into different coordinate systems. For the last installment, we’ll discuss how to scope results to nodes.

Node Interaction in Mechanical, Part 1: Picking Your Nodes

NosePicking1In version 14.0 of ANSYS Mechanical, ANSYS has rolled out its first capabilities for interacting with the underlying finite element model in addition to the geometry. In this version, the user can select nodes, create named selections from nodes, apply loads and constraints to nodes, and scope results to nodes. And it is glorious. In this posting, the first part in a four-part series on interacting with nodes in Mechanical, I will start of with the basics: selecting nodes in ANSYS Mechanical.

The default picking mode in Mechanical is to Select Geometry. In order to select nodes you will first need to display the mesh by either highlighting the Mesh branch or by clicking the Show Mesh (image) button. Next, switch the select mode to Select Mesh under the Select Type pull-down.

image

At this point you will be able to pick nodes in the same manner that you pick vertices. Note that the entity filter is automatically set to Vertex when you’re in Select Mesh mode, so you may need to reset the filter once you go back to Select Geometry mode.

image

You can also box select or lasso select nodes under the Select Mode pull-down. Note that there are two options for each: plain ol’ box and lasso select, and box and lasso volume select.

image

I’ve found that volume select vs. regular select is best illustrated using flat surfaces, so here we go: an example with flat surfaces.

image

Regular box or lasso select only selects nodes on the faces closest to the viewer.

imageimage

 imageimage

Note: To lasso select, simply click and drag the cursor around in a loop.

On the other hand, volume select selects all the nodes throughout the depth of the model.

imageimage

imageimage    

A related question that has come up when I demonstrate the new nodal interaction capabilities is, “Node numbers! Where are my node numbers? I want to see node numbers! Give me my node numbers!” OK, you can view node numbers now. (You can also view information about other entities, but this is a blog post about nodes, so I’m going to talk about nodes.) To view node information, first make sure you’re in node-picking mode, select the nodes of interest, and then click on the toolbar button featuring the blue ‘i’ with a black arrow next to it.  image (You can also do this in reverse order. Whatever floats your boat.) When you do this, the Selection Information will display the node X, Y, and Z location and Node ID in the lower left corner of the GUI.

image

If you had picked two nodes, it would also show the distance between those nodes. You can customize the display by clicking the green check box, though you probably won’t want to change anything with the node display.

In the next installment I will show you how to create nodal Named Selections starting with simple picking and moving on to such criteria as location, node number range, and nodes attached to solid model entities. This knowledge will come in handy for applying boundary conditions to nodes and scoping results to them, which I’ll cover in the third and fourth installments. Happy node picking!