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. The minutes were written for SolidWorks 2003.
30 people attended this meeting.
Click on links for easy navigation
Announcements—Moshe Saraf
- By
vote, we decided to extend the icon competition. Two entries have been submitted. A prize of a 256 Mb USB flash memory
drive has been purchased for the winner.
- We
reviewed the past year presentations and requested the user to submit
their preferred SolidWorks topics
- We reviewed meeting location and time preferences
Votes for meeting place
•
• De Pere 7
• Green Bay 7
• Any 1
• Total 30
Votes for meeting time
•
Average voted meeting time rounded to next half
hour -
In summary, we will continue to meet
at the Sports Corner in De Pere, and the meeting time
will stay at
- We are looking for users to present topics or share their SW design.
Beginner Tips – assembly mating – Moshe Saraf
Minutes prepared by: Moshe Saraf
Mate reference and SmartMates
were presented. Both aim at automating
the mating process.
Mate Reference
This feature allows you to specify mating information in a part. When this part is dragged into the assembly in the vicinity of certain model entities, “the software tries to find other combinations of the same mate reference name and mate type.” The pointer is changing to reflect the interpretation of the software for potential mate (see figure 1). And a shaded image of the part is shown in the mated orientation. When you let go of the mouse, the part is mated in the assembly. It may not put in all of the mates, but it can easily save on creating a couple of them per part. Note the orientation of the part before you let go of the mouse. You can flip to the back side by using the tab key.
Figure 1: Pointer icons
To insert a Mate Reference, click Insert and select Mate Reference… In the Mate Reference interface you are prompted to select reference entity from the model and the type of mate (figure 2). After selecting, a folder is created in the part FeatureManager Design Tree. You can add multiple mate references and name them uniquely.
Note that the information is kept with the part and adds to its file size. Mate References are recommended to be added only to parts that are repeatedly inserted to assemblies, such as screws and washers.
Figure
2: Mate Reference interface
Mate Reference to a slot
What mate reference do you use for a slot? Note that it is desired to have the screw or other part concentric to the tapped hole that in the part that the slotted part is fasten to.
We will talk about this in the March meeting. Please try and let us know if you have a solution.
Smart Mate
Similarly to Mate Reference, Smart Mate allows you to specify the mating entities by the way you click and drag a part.
a) Dragging a part into an assembly from another window
Open
the part to be mated. Open the
assembly. Click Window and select Tile
Horizontally. Select a model entity on
the part and drag it into the assembly.
The dragging process will be the same as in the Mate Reference. The part can be dragged into the assembly by
selecting a feature from the FeatureManager Design
Tree.
b) Moving a part in an assembly
Click
Move Component
,
Smart Mates 
,
and double click on a part entity
(figure 3). The part will turn
shaded. At the assembly entity, click
and hold the mouse. As you move the
pointer in the vicinity of the model entity, the pointer icon will indicate the
potential mate (figure 1). You may use
the tab key to flip the part over.
Figure 3: Move Component and SmartMates
Design Tables – Jeff Hallgren
Minutes prepared by: Bob Braun
Design tables can be used to control and create configurations in both part models and assembly models with an Excel spreadsheet. Use them for these reasons:
·
They are an efficient way to create and control
configurations.
·
You can use powerful Excel functions to drive
configurations. On pages other than the
first one, you can do design calculations that reflect directly into the
design.
·
The Excel spreadsheet of configuration
variations permits good record keeping.
If an unintended change is made, it can be reversed.
· Configuration details can be displayed in drawings for user information or for tabulated drawings. This will typically require some Excel format changes, probably including hiding some rows and columns of information.
Design tables can be created in any of three methods. The below list is in order of increasing frequency of use for most users and of increasing ease of use.
·
Manually create an Excel spreadsheet and import
it into SolidWorks.
·
Insert a new spreadsheet in SolidWorks
and use interactive functions to add details.
· Automatically create a new spreadsheet in SolidWorks based on the existing configurations (Must have two existing configurations to start). This is available in SolidWorks 2003 and more recent versions.
Select Insert Design Table from the drop down menu. The left illustration shows selecting the
design table from the drop down menu.
The illustration on the right shows the resulting message box.
In the message box, select the option button near the top for how you want to create your design table.
·
Select Blank
for a blank Excel spreadsheet that you can use to create your own design table.
·
Select Auto-create
to let SolidWorks create an Excel spreadsheet that is
already started (or completed) with the design variations in the configurations
that you have previously created.
· Select From file if you have previously created an Excel spreadsheet and you want it to control your configuration. This option is best used when you have a standard array of configurations that you would like to apply to multiple parts or assemblies in different files.
For most routine applications, most users will want to use the Auto-create option. It will provide the most efficient way to create most of the features that most users will need. Once the Auto-create option is used, the table can later be manually changed for special features.
The Edit Control and Options regions on the opening message box let the user manage how the design table will interact with the model. The tradeoff is that the more you limit the interaction, the less chance there will be of inadvertent changes and the greater your ability to reverse the changes while you also lose flexibility in how the design can be changed.
Here is a screen shot of a sample automatically created worksheet with a few superfluous columns hidden. Here are some things to note about this worksheet:
·
Column A has the configuration names.
·
Rows 3 and below are each for a separate
configuration.
·
Cell A2 is blank. While inserting rows above it for
documentation may push down this blank cell, it must be blank.
·
Columns B through I in this test part are custom
properties that can be edited in this worksheet.
· Columns J through N are custom dimensions for each part configuration. When these dimensions get renamed to more meaningful names than D1 and D4, for example they can be named as Length and Width, those names will carry over to this worksheet. Only those dimensions that are configuration specific are listed.
Additional configurations can be added by populating additional lines in the worksheet. In this example, copy line 3, 4 or 5 to row 6 and edit the copied values to match what you would like. If you want to drive the configurations based on calculations or links to other documents, use the first worksheet page only for the configuration specifications. Use subsequent pages or other documents for other elaborate calculations and make the result on the first sheet equal to the desired calculated value. SolidWorks works with the displayed value.
Design tables permit you to control these configuration features:
·
Dimensions
·
Suppression states
·
Hidden states
·
BOM value display
·
All custom properties
·
Derived configurations
·
Equations
·
Relationships
· In assemblies, component states and configurations used.
Here are some additional related details from the presentation.
·
Use the dimension properties to assign a meaningful name to a dimension. Right click on the dimension and select Properties from the drop down.
·
In order to see dimension names, go to the Tools|Options
menu. Under the System Options tab and with General
selected, select Show dimension names. This setting will sustain across your local SolidWorks program until your reverse it.
·
You can automatically enter
additional dimensions by double clicking on the desired dimensions when the
design table is open. Note that the
active cell in the Excel worksheet must be blank and in the parameter row.
·
You can manually enter additional dimensions (or
create a table from scratch) by labeling additional columns with the format of dimension name, the @ symbol, then the feature name, typically
“Sketch<n>” unless the feature is not a sketch or it has been renamed.
· When you want to edit the design table, right click on the Excel icon in the menu tree and select Edit Table or Edit Table in New Window.
Physical Simulation – Mike Jagemann
Minutes prepared by: Moshe Saraf
Physical Simulation allows you to simulate the effects of motors, springs, and gravity on your assemblies. The simulation uses the assembly mates and physical dynamics (collision between solids) to move components in an assembly. It enables recording, replaying, and saving the simulation with the file.
How to find the
physical simulation?
Right click on any tool bar and check Simulation (figure 4).
Figure 4: Simulation tool bar
How to create a
simulation?
Select an actuator.
An actuator can be a linear motor, rotary motor, spring, or
gravitation. The pop up window will
prompt you to select model entities and to set the critical parameters. Then, click Record Simulation
. Stop the recording when it reached your
desired length.
Managing the
simulation
When creating the physical simulation in an assembly, a folder is added in design tree. The folder contains the actuators and the replay. As with other features, the Simulation folder or the actuators can be suppressed. Also, actuators’ definition can be modified.
How would I export an
AVI movie?
To
record an AVI movie, use a screen capture software while playing the
simulation. SolidWorks
Animator has a screen capture feature.
Without screen capture software, you will only be able to look at the
animation on your screen.
How does the
simulation behave with collision?
Since the Physical Simulation is based on Physical Dynamics, it will stop at collision, and will prompt you with a message if it starts at a collision.
What are the
limitations?
Ø The simulation is not a dynamic analysis. Kinematics, friction, deformation of bodies, and reaction forces are not calculated.
Ø Motion is not continuous and is based on recording small steps of the Physical Dynamics feature. The size of the steps is defined by the sensitivity slider in Physical Dynamics (figure 5).
Ø All actuators start at time zero. Physical Simulation does not allow you to delay actions.
Ø Actuator’s speed is linear.
Figure 5: Sensitivity in Physical Dynamics
Examples
To review examples of such simulations click the following link. http://www.mikejwilson.com/solidworks/solidworks_files-03.htm and see Physical Dynamics. The movie of that example demonstrates what can be done with physical simulation.
Next meeting
Our next meeting is tentatively scheduled to
Tentative agenda
- Announcements
- SolidWorks world report
- SolidWorks Best Practices and Standards overview
- light meal
- SolidWorks Best Practices and Standards at several companies in the area
- Panel discussion of SolidWorks Best Practices and Standards
- Icon competition
Please contact the board if you have anything to share about best practices and standards. Also, contact the board if you are interested in presenting your company’s SolidWorks standards or be on the discussion panel.