NEWSUG Meeting Minutes
Sports Corner, Depere
While this report generally covers the meeting events, they have been arranged into a logical sequence and refined with the purpose of making them helpful without necessarily precisely representing the facts as they happened.
24 people attended this meeting.
Click on links for easy navigation
Announcements—Moshe Saraf
· NEWSUG icon competition on December 3rd – please submit your icon model and win a prize. For example, see the following icon:
Guidelines are published on the web. This is a great opportunities to show your skill, creativity, and involvement in the user group activity.
·
NEWSUG new e-mail – newsug@newsug.org
· NEWSUG web site improvements – the site appearance and organization was improved by Mark Achtner. Specifically, look at the link page. Good job Mark.
· Combined SolidWorks user groups meeting on Thursday September 18. For details and registration click Combined User's group meeting.
· Additional board member is needed to share the load, to allow a more diverse representation from different companies, and to generate more involvement.
· NEWSUG Charter change – to be able to add a board member the “Three board members” phrase in the charter was voted by the group to be changed to “At least three board members”. See updated charter.
Beginner Tips – assembly mating - Moshe Saraf
Assembly mates are needed to locate a component in an assembly space and to fix the component’s degrees of freedom.
· Productivity
Ø Use only enough constraints to functionally control the model. Avoid constraining the same degree of freedom with multiple constraints like both a parallel constraint and a coincident constraint. Do not bother to restrain the angular orientation of cylindrical parts where orientation does not matter, like cylindrical bushings and threaded fasteners. This will minimize user effort and SolidWorks solve time.
Ø Cubic models require three mates to fix all degrees of freedom
Ø Cylindrical models require two mates to fix the major degrees of freedom
Ø Always start with the concentric mate because it fixes two degrees of freedom in one mate.
·
Mating scheme
Ø Intuitive mates - make intuitive mates, so users that will use your assembly models will easily understand how a component was mated. What are intuitive assembly mates? In general, use the surfaces that need to be in relation in the real world. For example in coincident mating, select the two surfaces that are in contact. Think of the motions that an assembler does when assembling the two parts.
Ø Skeletal mates – this will be shown in our next meeting.
·
Model entities selection
Ø
Hold the CTRL key and select the two surfaces. Then click on the mate icon 
that is in the assembly toolbar
.
Ø Click on mate first, and then, select the model entities.
Ø
To select a surface that is hidden, use Select
Other. Right click on the model, and
select Select Other.
The cursor will change into 
. Every right click (N
for no) will highlight a different surface.
Once the desire surface is highlighted, click the left mouse button (Y
for yes). In most times, SolidWorks will start highlighting the correct
surface. This can save you from having
to manipulate the component.
·
Viewing the mates
Ø Right click on the model and select view mates
Ø Right click on the assembly at the top of the Feature Manager Design Tree, select view dependencies, and click on the + sign by the model of interest. Note that in SolidWorks 2004 every component in the assembly has a mating folder in its design tree. Also, the View Dependencies does not exist in SolidWorks 2004.
Large Assemblies—Greg Jankowski
A large assembly is any assembly that is complex enough to tax your system and be a detriment to productivity. Click here to download Greg’s large assembly power point presentation.
SolidWorks
2004
There many new functions in SolidWorks 2004 to aid the creation of large assemblies.
· You can now open a sub-assembly as a lightweight component.
· The display of the Feature Manager design tree using the View Dependencies command has been enhanced.
· No need to save eDrawing data with your file. EDrawings will view any SolidWorks document without it saved
· You can suppress or edit mates and view multiple sets of mates with errors in the Mate Diagnostics Property Manager.
· The Mate Property Manager is enhanced to sort standard mates from advanced mates, allow editing of multiple mates at one time, and so on.
· You can copy and print the list of referenced documents in the Search Results dialog box.
PC Hardware
The amount of RAM and Processor speed are the two major components that will affect assembly performance. Other tips are listed below.
· RAM
o If your computer is accessing virtual RAM, then you need to add more RAM to your system. To check you virtual RAM usage use “ctrl-alt-del” to access the task manager, as seen below. Then open up your largest assembly and a few parts. If your available memory is low, then you should add more RAM.
o Do not let your computer use virtual RAM.
o Adding RAM is inexpensive and can greatly improve your system.
· Processors
o The speed of your processor is very important. The faster the processor the better the assembly performance.
o Two processors will bring only about 5-10% performance gain. SolidWorks does not multi thread instructions and thus does not take advantage of a dual processor system.
An unrelated topic
It was noted that SolidWorks 2004 will support NT and ME, but the next version of SolidWorks will not support NT or ME.
SolidWorks
Settings
Adjusting your SolidWorks settings can provide improved assembly performance. The settings can be accessed by clicking on tools menu and then options. For more info see the Best Practice guide in the Support section on the SolidWorks website. Log into the support section and then click on guides which is located on the left side of the screen.
· Image quality
o Image quality is located in the Document Properties tab.
o Set the image quality settings as low as you can tolerate.
o Image quality can gain you up to 10% in performance.
· Performance setting
o Performance is located in the System Options tab.
o Turn on the automatically load components lightweight. This option can greatly improve opening and assembly and performance.
o Click on remove detail during zoom/pan/ rotate to improve performance.
· Large assembly mode
o Large assembly mode is located in the System Options tab.
o There are a number of settings in this section to improve performance.
· Drawings
o Drawings is located in the System Options tab.
o Turning off the Allow auto-update when opening drawings will increase performance.
o Turning on Automatically hide components on view creation will also increase performance.
· Miscellaneous settings
o In the sketch setting, which is located under the system options tab, check use fully defined sketches. Undefined sketches can decrease performance and take longer to build.
o Change the file location of the Journal file to a location on your local hard drive. If the journal file is located on a network drive it can decrease your performance.
Modeling Techniques
Planning the way that you model a part can improve assembly performance.
· Combining similar features decreases the time to rebuild a part and assembly.
o Combine similar fillets. Alternatively, If you have difficulty filleting a part, try a different filleting order. A different filleting order will sometimes allow you to achieve a difficult fillet.
o Combining too many features can cause problems when suppressing or designing a part.
o A balance between combining similar features and keeping other features separate is the goal.
· Decrease complexity in a part will decrease the time to rebuild a part.
o As an example you do not need to draw the threaded portion of a screw. This can be simulated with a just a cylinder. Avoid unnecessary detail.
o Avoid using text as a feature.
o Avoid using lofts, sweeps and helixes.
o If you do need detail in a part, create two configuration of the part. One configuration would be a simple version and the other the detailed version. Use the simple version in an assembly to improve performance.
· If you are pattering a feature. Try using the geometry pattern.
o Geometry pattern has been greatly improved in SolidWorks 2004.
· Resolve any errors or warnings. Errors and warning increase the time it takes to rebuild a part or assembly.
· Turning on the name feature on creation will make for a clean feature tree. If you need to make a modification to the part at a later date, it will make it easier to remember how the part was modeled.
Assembly Performance
Planning the way you create an assembly and utilizing certain features in SolidWorks can increase assembly performance.
· Open parts in lightweight that you do not plan to modify.
· Use the save assembly as a part for subassemblies.
o This can be used to create purchased subassemblies.
o This will decrease the time it takes to rebuild a part.
· Use configurations.
o Create a configuration with all of the parts and one with only the parts that you need to work on.
o When you open an assembly, you can choose which configuration to open. Choosing the correct configuration to open can improve time to open.
· Do not use the flexibility function in a subassembly if you do not need it.
· Avoid using excessive patterns.
· Mates
o Mate to logical components and robust features whenever possible
o Mate as high as possible in the tree
o Minimize (sensible) In context features
o Minimize mating to in context features
· Using a skeleton can improve assembly robustness.
o A skeleton is a combination of planes and assembly sketches. You can mate your parts to these planes and assembly sketches.
o Mating the planes of a part to the skeleton will decrease the risk of a mate breaking when a part is modified.
Drawing Performance
· Lightweight
o Use lightweight when opening a drawing that contains an assembly.
· Detachable (Rapid Draft)
o Rapid draft drawing are now called detachable drawings in 2004. Detached drawings are similar to rapid draft. But, now you can reattach a detached (Rapid Draft) drawing.
o A detached drawing will not rebuild the part every time. It will only prompt to be rebuilt if the assembly has been modified.
· High Quality and Draft Quality
o Use shaded previews to decrease rebuild time.
o In the System Option Settings select Always Automatically convert drawing views to draft quality when unloading components
· Use Hide/Show Components to hide internal detail other performance options
COSMOSXpress, part
II—Bob Braun
COSMOSXpress is a subset of Cosmos Works, a solid entry level FEA package. The benefits of COSMOSXpress are that it is free with SolidWorks and it is easy to use. The limitations of COSMOSXpress are:
·
The only quantitative output is VonMises stress.
·
The only kind of constraint is a fully
constrained surface.
·
The only kinds of loads are normal to a plane or
surface.
·
Only solid elements can be used.
·
COSMOSXpress only
works on parts, not assemblies.
· Users cannot see the mesh to validate it.
We reviewed these points from the May meeting.
·
We need to be careful to not overly constrain
the part by the way we assign restraints to the model. This can result in modeling errors because it
artificially projects the stiffness of the supports on to the part and the part
on to the supports.
·
In tight corners, excessive element size can fail
to show the true stress.
·
Assemblies can be converted into parts for COSMOSXpress analysis with a technique detailed in the May
minutes. In the presentation on large
assemblies, we discovered a technique for saving the assemblies that may work
to convert them into parts.
·
Use split lines to divide a surface for more
precise load application areas and restraints.
·
Routinely reduce the tolerance size by two or
three orders of magnitude in order to minimize problems with getting solutions.
·
Choose your input and output units, as well as
the location of temporary files, in the options
command button on the first tab screen of the wizard.
· Add needed planes to define the load direction.
We briefly discussed welds. Welds present a severe modeling and analysis challenge for any software package. This advice was given:
·
Design to avoid welds in areas of significant
stress.
· Identify a company internal expert who is responsible to research and analyze the specialized area of welds.
The angle bracket presentation was repeated with these additional tips.
·
Make corners in high stress areas accurate, not
dead sharp, in order to get helpful stress results.
·
Match your element size to the smallest feature.
· Model simple parts with known results in order to become familiar with the software and to get the needed background on how to size your elements.
We did an exercise with a cantilevered beam 1 X 1 X 10 inches long with 100 pounds of force on one end. We solved this beam with a variety of element sizes from 1 inch and smaller. This is what we learned:
·
All element sizes resulted in a calculated
maximum stress with less than ten percent error. As far as modeling goes, that is reasonably
good.
·
With element sizes smaller than ¼ the beam thickness,
we started to model how the beam was made more rigid by its support and not
just the bending stress, which is the classic calculation. In other words, since FEA answers more than
the obvious question, you do not necessarily get the obvious answer. This is an excellent learning experience
about how stress is really distributed in a beam.
· In order to get the load to be applied parallel to a surface, you need to pick both the surface that you want to apply the load to and the plane that you want the load to be normal to. There is a small difference between how this is done in SolidWorks 2003 and SolidWorks 2004.
Since COSMOSXpress only permits you to constrain a part on a surface, this sometimes will overly constrain a part and give false answers. A work around was demonstrated in which flexures were created to support the part. A flexure is a thin beam that has high rigidity in compression (and tension) but is flexible in one direction (for small displacements) and typically has medium rigidity in another direction.
The conclusion of the presentation is the COSMOSXpress is a low cost solution with substantial limitations but the ability to get valid answers to some questions if you use it thoughtfully.
Next meeting
Our next meeting is tentatively scheduled to
Tentative agenda
Announcements
Beginner's tips - Assembly mating continues
Design tables
Break
SW simulation
Icon competition
We are looking for users to share examples on these topics.