Miller Electric,
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.
22 people attended this meeting.
Announcements — Moshe Saraf
·
We are having a contest to come up with a NEWSUG
logo. The design must come from a NEWSUG
member and it must be modeled in SolidWorks.
Contest guidelines will be available by the next meeting.
·
We are looking for presentation volunteers for
future meetings.
·
SolidWorks is looking for beta testers for
SolidWorks 2004. This will be done
around September 30.
·
Next meeting is tentatively scheduled for
Beginner Tips — Moshe Saraf
File Management
Three approaches to file management were discussed, at least briefly: PDM software is the most powerful approach. When a company has many SolidWorks seats, PDM software is the only reasonable option. SolidWorks Explorer covers basic file management requirements of moving, copying and renaming files. These file management tasks can be accomplished also within SolidWorks. The notes below will focus on how to accomplish several basic file management tasks. Please refer to the help sections in SolidWorks and SolidWorks Explorer using the key words in the titles.
|
|
To rename files in assembly or assembly drawing
This will create a copy of a component file with a new name, which will be referenced in the assembly. Save as… method
|
|
|
SolidWorks Explorer method
|
To replace a component in an assembly drawing
This will replace a component in an assembly drawing while modifying the reference of that component in the drawing references.
Save as… method
- With the assembly drawing open is SolidWorks, click File
- Select Save as…
- Click References…
- Check the component to be replaced
- Double click on the path of the component to be browse to the replacement part.
- Click Open.
- Click OK.
- Click Save and Yes when you are asked, “Do you want to replace it?”
SolidWorks Explorer method
- With the assembly drawing closed in SolidWorks, click Browse… and select the assembly drawing.
- Right click on a component and select Replace.
- Click Browse… and select the replacement component.
- Click Apply.
|
|
To copy a drawing or an assembly with all references
files into a new folder
This will copy the drawing or the assembly with all its referenced components into a specified folder. Save as… method
|
|
|
Find References… method
SolidWorks
Explorer method
|
Note that majority of users use SolidWorks Explorer for file management. SolidWorks Explorer provides an interface with many file management functions, so several tasks can be accomplish on one screen.
Back to the Top of the Document
COSMOSXpress — Bob Braun
We started with an overview of what FEA
is. FEA is a math intensive technique
used to solve problems that are too complicated for textbook formulas. An entire part is broken into elements that
are simple enough for general solutions.
With modern software, most of this work is automated.
Typical entry level FEA solutions can be used
to calculate various types of stress and deflection as well as do modal
analysis, buckling and thermal analysis.
Boundary conditions are FEA speak for loads and constraints on a
part. A good general FEA package will
permit a wide variety of useful ways to apply the load and restrain the part
that are good approximations of the actual ways the part interacts with the
world. A good general FEA package will
also have a variety of element types that will let you model part behavior with
ease, accuracy and in a format that permits rapid problem solution.
While Cosmos Works has many, but not all, of these features, COSMOSXpress has a far more limited feature set. The trade off is that in exchange for an attractive price (free with SolidWorks 2003) and an easy to use interface, you get severely limited functionality. It is wizard driven with intuitive navigation. The only available boundary conditions are fixed surface and force or pressure normal to a surface or plane applied to the surface. The only outputs are VonMises stress and general deflection shape. You have no option to select element types, see the mesh or get quantitative deflection information.
You can access the COSMOSXpress help topic by selecting COSMOSXpress, under the Tools menu, and selecting the help command button. This section gives some of the assumptions about analysis, using COSMOSXpress and contrasting COSMOSXpress to Cosmos Works.
In a demonstration, we learned:
·
When you have a part
designed, select COSMOSXpress under
the Tools menu. This will bring up a wizard that will walk
you through the analysis process.
·
Configure COSMOSXpress
for the units that you want and where you want to store your analysis files with
the Options command button on the
COSMOSXpress opening screen.
·
Thoughtfully take out
small features in order to get faster solution times.
·
Use split lines to
help create more realistic boundary conditions.
Create a split line with these steps:
1. Open a sketch on the desired split surface.
2. Sketch the desired shape of the split line contour. In the demonstration, we used circles around
attachment points.
3. With the sketch open, on the Insert menu, select Curve
then Split Line.
4. Select that surface that you want to be split.
While COSMOSXpress encourages the user to
accept the default element size, Bob encouraged you to select the option button
to change the analysis settings. While
the program will often make a reasonably good choice about element sizes, the
tolerances often need adjustment. The
tolerance defines the size of a sphere around each element node. If more than one element fall into a common
sphere, they will be merged. This is an
effort to avoid cracks in the FEA model.
What often happens is that two nodes from the same element fall into the
same sphere and are merged. The result
is a fatal error because of the badly shaped element. The solution is to make the Element tolerance smaller by a factor of
100 or 1000. Solution time is sensitive
to element size but not to element tolerance.
Cutting the element size in half will generally make the problem take at
least eight times longer to solve.
Because Cosmos uses relatively sophisticated elements, we usually get
good results with a relatively coarse mesh.
Reducing the tolerance size will not significantly change solution
time. When FEA models fail to solve,
this is one of the first places to start changing things in order to make them
run.
COSMOSXpress does not work on assemblies. In order to do an analysis of an assembly,
you need to merge the assembly parts into one part and solve it. Here are the steps to do that:
1. Open your saved assembly.
2. On the Insert
menu, select Component then New.
Enter a name for the new part and select save.
3. On the Insert
menu, select Features then Join.
4. In the feature manager design tree, select the components
that you want to join. Their names will
be listed in the dialog box.
5. Make sure that the check boxes for Force surfaces to surface contact and Hide parts are checked.
6. Select the OK
check box to close the dialog box. Your
part will now be available and linked to the assembly.
Back to the Top of the Document
The help menu also contrasts the two methods in Comparing Sheet Metal Design Methods.
Both are valid and are still fully supported with advantages for each but most advantages fall on the designing with sheet metal method. The main difference between the methods is that in the convert method you create what you need and then unfold it. In the create method, you create the part as a sheet metal part. The methods can also be combined. Part of the presentation is how to unfold the whole part or how to unfold selective bends and how to refold the whole part.
In addition to designing with sheet metal, Mark demonstrated creating and using forming tools. Mark recommended that each company create its own library of forming tools. A forming tool is a SolidWorks solid model that is used like a forming tool to either form or form and cut a shape in a sheet metal part. The procedure is covered in the help menu under Using Forming Tools with Sheet Metal and links from that help topic. In summary, a forming tool is a SolidWorks solid model that is the male die that could be used to form a sheet metal stretched feature like a louver or extruded hole. All features must lie below the model’s horizontal plane. In order to cut an opening with a forming tool, color the surfaces in the forming tool with the color Red 255 while Blue and Green are 0. Forming tools can only be accessed from the feature palette.
Mark reviewed these tips and tricks:
§
Manually select the width and depth for the
relief for each bend. The SolidWorks
default uses a formula based on material thickness that will likely result in a
notch specification that your shop is unlikely to have tooling for. If the part is laser cut, and not hard
tooled, the SolidWorks defaults will be fine.
§
Create a jog or offset in a part by sketching a
line on a surface and choosing the Jog
button. This topic is covered in detail
in the help menu under More Sheet Metal
Topics.
§
Use the Hem
tool to make sheet metal hems efficiently.
§
It is advised to create the flat pattern after
the part has been completed. It can be
created automatically or manually. If
you create it manually, it will be a derived configuration. Making flat patterns is covered under the
help menu under More Sheet Metal Topics. After making the flat pattern be sure to
verify that the flat pattern represents the part that you want.
§
Be careful when adding features after the
process bends. If you dimension them
inappropriately, they can move unexpectedly when the flat pattern is made.
§
If you create a part using the base feature, you
cannot use the insert bends feature later in the part.
§
If you create a part using the insert bends
feature, you can use the other tools to create a combination part.
§
Unsupress the flat pattern feature to flatten a
combination sheet metal part.
§
Rather than add fillets to all corners, use the Break-Corner/Corner-Trim icon.
§ In your flat pattern drawing, you can show or hide the tangent lines for the bends in order to make your bends visible or invisible.
Miller Electric Sheet Metal Tour—C. J. Philipsen
The group took a tour through Miller Electric sheet metal forming, cutting and welding departments as well as painting and some assembly operations.