December Tech Tips
Customize Mouse Gesture tool bar: You may have
heard of the new mouse gesture activated shortcut in SolidWorks
2010. It is activated by holding down the right mouse button, and
dragging the mouse to the right. A donut shaped shortcut tool will
appear that can be customized to your liking. By default, the donut
will have 4 shortcuts on it, but that can be customized to 8.
Customize the mouse gesture shortcuts the same way you customize
any toolbar in SolidWorks, which is by right clicking over a fixed
toolbar and selecting "Customize". There is a new tab in the
customization dialog now titled "Mouse Gestures" From there, you
can add your own choices of features and tools to the gesture based
popup, which is context sensitive. For even more choices than the
maximum of 8, you can add a shortcut to the shortcut toolbar
normally activated by the "S" key.
Parametric Text Notes in Sketches: In
SolidWorks 2010, you can now link a text note in a sketch to a
custom property. When adding a text note in a text, just click on
"Link to Property" in the property manager of the text being added.
From here you can link to either a custom property, or a SolidWorks
Special Property like the configuration name. With this method, the
text, and any feature that is created from the sketch it resides
in, will update every time the property changes. This a great
technique for cases where a property like a part number or mold ID
number needs to be molded or cast into a part.
Technical Resource Document - SolidWorks Rx:
SolidWorks Rx is a troubleshooting tool that SolidWorks includes to
give you first-pass, diagnostic information about your SolidWorks
usage. For complete instructions - visit our technical
resources page.
November Tech Tips
Midplane End Condition with Instant 3D
When creating an extrusion by dragging the green arrow, hold down
the "m" key to switch to a Midplane end condition. This only works
if you are using Instant 3D and creating a feature by selecting the
green arrow that is available after selecting an unabsorbed
sketch.
Isometric Section View in Drawing
Ever want to show a section view displayed in an isometric view?
This is simple to do and gives your drawings the real feel for your
parts and assemblies. Create a section view like you normally would
and then right click on the new view. You are given the option
"Isometric Section View," select this and it will change it into a
3D view. If you don't like it, right click again and "Remove
Isometric View."
October Tech Tips
Free Structural Members for Weldments
SolidWorks' Weldments can use a sketched "wireframe"
representation of a welded structure, and then apply industry
standard structural shapes (beams) to the wireframe sketch
entities. But, "of the box" we only get a few examples of the type
of profiles used with the Structural Member tool (ansi & iso,
angle, rectangular tubing, channel). Instead of creating the
missing structural profiles you need, there are extensive libraries
freely available for download directly from the Design Library.
Under SolidWorks Content -> Weldments you will find links to
profile libraries defined by ANSI, ISO, DIN, JIS and others
including Unistrut. Unzip the contents of the downloaded file(s)
and include that folder under File Locations -> Weldment
Profiles. The scope of these libraries is impressive. ANSI has over
2000 profiles including steel & aluminum, wide flange, T
sections, MC channel, pipe, and much more.
Gauge Tables Reduce Errors
Gauge tables are simple spreadsheets used by Sheet Metal that can
impose manufacturing or company standards for material thickness,
allowable bend radii and bend allowance technique. Typically
applied through the Base Flange command, once a gauge table is
selected any Property Manager fields that require input values then
change to drop-down pick boxes. Now, unless you override the table,
you can no longer key in a non-standard material thickness. Also,
for any allowable thickness you must select an allowable bend
radius, unless you override the table. Create gauge tables for
specific materials (304SS vs. copper) or bending techniques (air
bending vs. bottoming), different machines, customers or vendors.
Check out the examples found in \lang\english\Sheet Metal Gauge
Tables. Be sure to include the path to your saved tables under File
Locations -> Sheet Metal Gauge Table.
Mouse Gestures
New in SolidWorks 2010 is Mouse Gestures. You can use a mouse
gesture as a shortcut to execute a command, just like a keyboard
shortcut. To activate a mouse gesture, just right-drag your mouse
and the guide will appear showing the command mappings for your
gesture direction. This can be customized for up to eight gestures
for drawings, assemblies, parts, and sketches. To view or edit the
current mouse gesture assignments, click Tools > Customize. From
the Customize dialog box, select the Mouse Gestures tab.
Add a plane even quicker
You can quickly add a plane without going to Reference Geometry.
All you need is an edge. Add a plane normal to edge by simply
clicking the edge, then clicking Insert > Sketch. This will open
a sketch on a newly added plane that is normal to the edge at the
closest edge end point.
September Tech Tips
Speedy Sketching
Ever wonder what Rapid Sketch does? So did I! This command can be
turned on from the Sketch toolbar to blaze through sketch creation
faster than ever before. Once activated choose the sketch tool of
your choice and then hover over any planar face in your model.
Start sketching once you see the Rapid Sketch plane appear. No need
to exit sketches or change tools when moving between separate
sketch planes, just hover, sketch and repeat! All the sketches are
immediately saved in the FeatureTree as soon as you start
another.
Sketching With Style
The Power Trim function of the Trim command tool does a lot more
than just trim like a scalpel. The real "power" comes from the
lesser known artistic abilities. With Power Trim active left click
and hold on a sketch segment and pull in either direction to gently
trim or extend.
Weldment Groups
You can now define a weldment group, a collection of related
segments in a structural member. Configure a group to affect all
its segments without affecting other segments or groups in the
structural member. You can define a group in a single plane or in
multiple planes. A group can contain one or more segments. A
structural member can contain one or more groups.
Escape Key is a Time Saver
You can press 'Esc' to interrupt long operations such as drawing
view creation or long drawing document rebuilds. The operation will
immediately cease so that other operations can be completed.
August Tech Tips
Customizing Hole Notes
The Hole Wizard can be a useful tool, unless it's notating your
holes incorrectly. This tip will describe what to look for and
links to resources that will assist in customizing your hole
annotations. Look for the file calloutformat.txt located in
C:\Program Files\SolidWorks\lang\english directory. There are two
versions of the file within this directory, calloutformat.txt and
calloutformat_2.txt. calloutformat_2.txt is easier to understand.
This file allows you to customize the order the variables in the
hole note are written in, add/remove variable information, and
adjust text values. Once the file has met company standards, simply
place on a network location and point all Solidworks client
machines to that file using the tools/options/File Locations
pulldown from within Solidworks.
Adding a quick light source to a part
By splitting faces on components, you can assign specific
appearances to an individual face. Then, with the PhotoWorks add in
turned on, apply an appearance to the split face, select the
advanced tab at the top, select the illumination tab and a constant
option, adjust brightness as necessary. When rendered, these can
produce great looking LED strings or other luminescent features.
Great for Marketing and Sales!!!
July Tech Tips
3D Content Central for free add-ins
I'm sure everyone at some point has thought "surely other people
need a feature in SolidWorks that does <insert your favorite
item>." The good news is that there is a place where you can
search for solutions, www.3DContentCentral.com. Many people are
aware that this site has many parts and assemblies, both from other
users and also certified by vendors.
This particular tip is referring to the macros on that site.
I'll state first off that the macros are not tested by SolidWorks,
so be careful what you download. With that out of the way, a
particularly handy macro allows you to find the mass of an
individual component in an assembly. www.3dcontentcentral.com
To use this macro, select a component, then run the macro. A
popup dialog box will show you the selected component's file name,
configuration name and mass (in kg). With very little effort, the
macro can be edited to display the mass in lbs or any other
preferred units.
Ok, so you can do this all through the existing interface, but I
wanted to bring attention to 3DContentCentral's list of macros in
hopes that many of you will use it and add to the list of
macros.
So, you're asking how to find a component's mass from an
assembly? Simply click Mass Properties, then in the Selected Items
box, right click to clear the assembly from the list and select any
component you want to analyze. Once you click Recalculate, you'll
see the mass, volume, surface area and everything else you're used
to seeing.
Component Configurations in a jiffy
Adding configurations to parts is easy to do, but what if you need
create the same configuration in an assembly and then activate the
part's new configuration? The simplest way to accomplish this is
from the assembly. As an example, we'll walk through creating a
configuration called Simplified to multiple components at a
time.
Open an assembly in SolidWorks and go to the Configuration
Manager. Right Click on the top entry and click Add Configuration
which will naturally add a configuration to the assembly. Name the
configuration "Simplified" and before you click OK, scroll down to
the bottom of the Property Manager to the Parent/Child Options.
Expand this section to see all the components of the assembly
(parts and sub assemblies). Place a check next to each component
that needs a Simplified Configuration. If you choose to check a
part that is part of a subassembly, be sure to check the
subassembly as well. Once you click OK, you can then click on the
Feature Manager and will notice that all the components selected
(and the top level assembly) have the new Simplified configuration
active. Open or edit each component and modify it as needed.
Instant 3D Modify Dimension Dialog Box is
Reduced
If you have instant 3D turned on then when you click on a
dimension only once it shows a reduced dialog box that only allows
you to change the dimension. If you want to bring up the regular
dialog box, double click on one of the blue dots associated with
that particular dimension and it will bring up the regular modify
dimension dialog box.
Purple Dimensions
From time to time everyone needs to create a cut. Have you ever
left the sketch under defined for the one edge that is away from
the part? Sure, everyone has! Why do you leave it under defined?
Well that's because when you create a drawing and import the model
items, you don't need that dimension to be shown on the drawing so
you leave it off. The best practice is to throw a dimension on the
entity and then uncheck the button "Mark dimension to be imported
into a drawing." This turns the dimension purple and allows you to
fully define your sketch.
June Tech Tips
Bi-directional Material Property Editing from Title
Block
I'm sure everyone at some point has thought "surely other people
need a feature in SolidWorks that does." The good news is that
there is a place where you can search for solutions,
www.3DContentCentral.com. Many people are aware that this site has
many parts and assemblies, both from other users and also certified
by vendors.
This particular tip is referring to the macros on that site.
I'll state first off that the macros are not tested by SolidWorks,
so be careful what you download. With that out of the way, a
particularly handy macro allows you to find the mass of an
individual component in an assembly. www.3dcontentcentral.com To
use this macro, select a component, then run the macro. A popup
dialog box will show you the selected component's file name,
configuration name and mass (in kg). With very little effort, the
macro can be edited to display the mass in lbs or any other
preferred units.
Ok, so you can do this all through the existing interface, but I
wanted to bring attention to 3DContentCentral's list of macros in
hopes that many of you will use it and add to the list of macros.
So, you're asking how to find a component's mass from an assembly?
Simply click Mass Properties, then in the Selected Items box, right
click to clear the assembly from the list and select any component
you want to analyze. Once you click Recalculate, you'll see the
mass, volume, surface area and everything else you're used to
seeing.
Control Part Sizes Using an Assembly Design Table
Some top-down assembly designs may benefit from a design
table structured as a configurator that builds mating parts based
off direct, dimensional input. By first creating an assembly sketch
containing only construction geometry that has the dimensions
required to control the sizes of the parts, you can reference and
control the dimensions of the control sketch in the assembly design
table, enabling a convenient way to configure all the required
component sizes easily from the assembly level. Use top down design
techniques like "Convert" and "Up to Vertex" end conditions,
referencing the control sketch when designing the parts top down.
The control sketch dimensions can then be controlled by the
assembly design table. Without this technique, The user must switch
back and forth between different part configurations to control the
various component sizes, making a much less direct method of
configuring the assembly.
Add an item to your design library
Have a commonly used part, sketch, assembly, or even feature? Add
it to your design library, making it easily accessible each time
you need to you use it. Your design library can be found on the
right hand side of your screen in your task pane. Verify your task
pane is visible under VEIW. Once in your design library you can add
either a folder or an individual file. If you add an individual
file you must add it to a folder in your design library. You can
also create a folder in your design library. Hover mouse over
design library task bar to choose your weapon of choice.
Standardize your company's part templates
Set your template for your company so there is no confusions about
what units to use. Open a new part under the templates tab of the
dialog box. Set your Document Properties under options. Save the
new template in a folder as a Part Template (*.ptrdot). To add the
folder to your template tabs, go to options and add the folder
under file locations, Document Templates.
May Tech Tips
Large Assembly Loading
lf you've ever needed to work on components in a large
assembly, but wanted the ability to make specific selections
without loading the entire assembly, you're in luck. When loading
an assembly from File, Open select the assembly, check off "Quick
view / Selective open" and then click Open. A graphical view of the
entire assembly will load in a fraction of the full load time.
Select the desired components to load into memory and click Open.
If you miss a selection, or would just like to open more parts,
click Show Hidden Components on the Assembly toolbar and choose the
additional components you'd like displayed.
RealView Rendering
Want to make your models and assemblies look even more realistic
without using PhotoWorks? Of course you do! Simply turn on RealView
graphics, along with Shadows and Perspective View (all of these can
be found under the menu View, Display). Next, change the scene to
Ambient Occlusion. While not in motion your models will be quickly
rendered using video game shading technology. For even better
appearance be sure to apply the appropriate materials to your
components and turn off any other on screen distractions like
origins or planes (View, Hide All Types). Please note - you must
have a RealView supported graphics card to take advantage of this
functionality. Visit www.solidworks.com to verify.
Customize your Keyboard
Commonly used tool can be linked to your keyboard so the tap of a
key will turn on your tool. My personal favorite is linking the
temporary axis to the T key. This customization can be used for
almost anything in SolidWorks to reduce mouse miles, from inserting
a feature to saving a file. Where to find: Tools, Customize,
Keyboard tab. Be sure to check your keyboard setting to maximize
efficiency and personalize your SolidWorks.
Clean up your Feature Tree
A large number of features can be a sight for sore eyes. Clean
your feature tree up by placing features in a folder so you can
find them with ease while editing. Right click on a feature, select
Add to New Folder. A new folder will be placed in your feature
tree. By default you will be asked to name the folder. To place
other features in that folder, just click and drag the feature into
the new folder. Remember, you can also name each feature and sketch
by slow clicking on the feature to edit the name. This will save
you time when editing parts.
April Tech Tips
Disabled Bodies in Flow Simulation
After Make use of disabled bodies in SolidWorks Flow Simulation to
focus in on detailed results in a particular area of your study.
Simply create a new part or body in your model, disable it from the
Flow study using Component Control, and then make use of its faces
and volume to display results in that area.
Equation-driven Motors in SolidWorks
Motion
Using expressions for motor definitions in SolidWorks Motion
allows you to create feedback loops. For example, you could use
this to maintain the velocity of a vehicle driving over a series of
hills at 10.0 m/s. First, create a result graph {linear velocity of
vehicle} showing the linear speed vs time. Next, define a motor
using an expression like; Motor speed = 10000 degrees/sec x
(10.0-{linear velocity of vehicle}).
How to move a group of sketch entities:
After creating a series of sketch entities you may want to move
the sketch entities around on the screen as a group. When
attempting to click and drag an entity you may notice that only
that entity will move leaving the other entities where you left
them. This often happens if there aren't enough constraints to hold
the entire sketch together. Here are a couple tips to help you move
under constrained sketch entities around the screen as a group.
Tip 1: Move Entities. Move entities allows you to pick
a group of entities and move them around. Using Delta X and Y
coordinates or by picking From/To locations.
Tip 2: Stretch Entities. Similar to Move entities,
stretch entities will allow you to move a group of sketch entities
but keep them attached to any entities that you did not select to
move. This will result in the entities between the moved and
stationary entities to stretch, hence it's name.
Tip 3: Align Sketch. It's in an unlikely location, but
the Align Sketch tool found on the 2D to 3D toolbar allows you take
all the entities in your sketch and map any point on that sketch to
the origin. Simply select a point on the sketch and click the Align
Sketch button.
Tip 4: Ctrl + Click-and-Drag. You may already know you
can copy sketch entities by highlighting them and clicking and
dragging the selected entities while holding the Ctrl key. But if
you let go of the Ctrl key halfway through the drag, you will move
the entities instead of copying them. Use this tip to your
advantage, it doesn't require you to click a command off a
toolbar.
March Tech Tips:
Creating Midpoint Reference Points on the
Fly:
The hard way to create a midpoint or reference point on a piece of
sketch geometry was to create a physical reference line or a
reference point in your sketches so you can dimension to that
midpoint. There is a better way though: when you are using the
SmartDimension tool you can right click a line (or other entities)
and choose Select Midpoint from the menu you are now able to
dimension to the midpoint.
How do you put a perspective view on a
drawing?
The traditional way to add "Perspective" within parts and
assemblies is not available within the drawing environment, but it
is still possible to place a perspective view into a drawing. To
show a drawing view with perspective, you will need to create a
custom view in the part or assembly file and that is the trick.
- Open the part/assembly file.
- Go to View, Display, Perspective.
- Zoom/Pan/Rotate to position the model as you wish.
- Hit the spacebar to bring up the View Orientation dialog
box.
- Click the icon that looks like a blue telescope with the sun
behind it. This allows you to save the current view settings in the
file. Type in a name for your custom view.
- Create or open a drawing of the part/assembly.
- Choose Insert, Drawing View, Model View, and choose your custom
view name from the list of possible views to place on the
sheet.
Do you use Excel and SolidWorks?
Not only can F2 rename a feature, sketch, configurations, planes,
etc. but it can also help inside excel. Take a look at a cell that
has a formula. If you want to edit the formula, typically you would
click in the cell and then click in the address bar. Next time you
need to edit the formula, move to the cell and hit F2. This will
take you to the end of the formula and allow you to start
editing.
Quick way to set the End Condition:
Whenever you are creating an extrusion (cut or boss) you have to
set your end condition (unless you are setting it to a blind depth
which is default). Instead of going to the property manager and
using the pull down, try using your Right Mouse Button and
selecting from the list displayed. This will reduce your mouse
miles significantly!
SolidWorks Explorer:
This tool is used to find references and rename SolidWorks files.
When you first start this program, it will ask you for your
PDMWorks user name and password. Some users might not be using this
function so is there a way to disable this from popping up
automatically? There is an option you can uncheck once you have by
passed that message and SolidWorks Explorer is running. The third
icon from the left is "Options." Once you have the options dialog
box open, select the "Add-Ins" tab and then uncheck the box next to
"SolidWorks Workgroup PDM."
February Tech Tips:
Input Dimension Value:
Designing in metric but thinking in inches? Try using the optional
dual units setting in the Measure tool. Just click the
Units/Precision button in the top header of the "Measure" dialog
box. Here, you will find the options for precision and custom units
settings in the Measure tool, including the "Dual Units"
option.
Dual Units in the Measure Tool:
Ever get tired of having to double click every new dimension in a
sketch each time one is placed in order to edit the dimension's
value? Try using the System Option "Input Dimension Value." This
option will cause the Modify box to open every time a new dimension
is placed in a sketch so that the value can be edited.
Convert to Sheet Metal:
The Convert to Sheet Metal command lets you specify the thickness,
bends, and rips necessary to convert a solid part to a sheet metal
part. This tool which combines the shell, rip and insert bends
command into one can be found from Insert, Sheet Metal, Convert to
Sheet metal.
Format Painter:
This tool has been moved from SolidWorks Utilities to the core
SolidWorks package. Format Painter copies visual properties from
dimensions and annotations to other dimensions and annotations in
the same document or another document. Format Painter is supported
by parts, assemblies, and drawings.
January Tech Tips:
Reuse your SolidWorks Motion Elements:
You can save motion elements such as springs, motors or force
specifications for reuse in other models. Add motion elements to
the Design Library as you would add other items. All motion
elements in the Design Library are saved with the .sldsimfvt
extension. While in any motion study, drag saved motion elements
from the Design Library to your model.
Make Complex Sketches Easier:
In SolidWorks 2009, you now have the ability to generate an
equation-driven sketch. The tool can be found under Tools, Sketch
Entities, Equation Driven Curve and the inputs required are an
equation and ranges for any parameters used in the equation.
Complex polynomials and harmonic equations can be easily used as
well allowing users to make very complex sketches.
Easier Appearance Manipulation:
In 2009, colors and textures have been combined in to what are now
knows as appearances. Because of this one source of display data,
factors such as RealView graphics and whether the model has been
rendered in PhotoWorks do not cause display information to be lost.
This leads to much easier application and manipulation of
appearances. Appearances can now be applied from the Appearance tab
in the task pane, the display pane or the Appearances selection
within any right-click menu.
Fully Define Sketch:
The fully define sketch feature allows you to automatically
generate relations and dimensions within a sketch. This is
particularly useful when 2D data has been imported in to SolidWorks
and you need the data to be fully parametric. This is also a very
useful tool when removing in-context references and still
maintaining the underlying geometry. The fully define sketch tool
can be found from Tools, Sketch Tools, Dimensions, Fully Define
Sketch.
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