Here's my two cents: Some tips are missing since they are only applicable to my company
1) To switch part creation plane from one to another:
1) Select the boss-extrude sketch
2) Right click and highlight "Edit Sketch Plane"
3) Dialog box comes up, select plane you want sketch to switch to, and apply
2) "ESC" exits from any function within SolidWorks
3) To select a face on the backside of model or part, click close to item you want to
select, Right click and highlight "Select Other" Use the Right mouse button to cycle
through and the Left mouse button to select.
4) To hide or show all dimensions, go to feature manager, Right click on "Annotations"
and highlight "Hide all Feature Dimensions"
5)With multiple drawings up, to switch between them without minimizing and
maximizing press "Ctrl Tab", this will cycle through the open drawings.
6) Smart Mating: To smart mate two parts, click on the smart mate icon, then DOUBLE
CLICK on the part you want to mate, it will become transparent, then drag it to the part
you want to to mate to.
7) from e-mail
Solid models require vast amounts of resources, including CPU time, disk swap
space, system memory, and display list memory. Model files can be and will become
quite large. These requirements are aggravated and made more excessive when you don't
keep models clean.
Unnecessary geometry is excess baggage that burdens you and others that work with your
models. If a model is not clean, the following problems can occur:
- Secondary models such as finite element meshes, STEP and IGES neutral files, and
rapid prototyping STL files have unnecessary elements and become more difficult to
control.
- NC tool path generation must process, ignore, and step over extraneous edges and
surfaces.
- Displaying the model becomes slower and inconsistent.
- Associative drawings may be incorrect, ambiguous, or undimensionable.
- The program may not specify tolerances and surface finishes properly.
- Model files become unnecessarily large, causing excessive loading, saving, and
processing times.
Clean models are more efficient and cause less work for downstream applications. Clean
modeling occurs when you follow a few simple guidelines:
- Create continuous surfaces that are not broken or trimmed unnecessarily.
- Delete excess geometry early and often.
- Always locate reference geometry such as profiles, reference lines, and templates on a
reference layer.
- Construct solids using the fewest steps.
- Avoid narrow faces and small corner angles that cause tolerance errors.
- Model files always contain a layer for designer's notes. Such information is invaluable
when you or others return to the model later for modifications.
- Avoid difficult geometry.
- Add before you subtract. Always perform Boolean adds (boss features) before subtracts
(cut features). This ensures that cavities and pockets are not filled in by mistake
9) When sweeping a complex shape use the sweep path if it falls on what will be the
outside of your part to cut away excess material before sweeping the profile.
10) Use symmetry about part origin when possible.
11) Rename critical features to make them easy for other people to find.
12) Use a rational order of operations, expecially if other people may be using
your parts. Reasons for transgressing this rule would be to accomplish a
workaround that because of a bug or limitation cannot be done a better way.
13) Separate holes into different features to make suppressing them individually
possible. Don't create holes by making nested extrude sketches.
14) "Multiple radius" fillets promote poor design practice. Use "constant
radius" fillets where all fillets created by a single feature have the same
radius.
15) For mold and plastics design, to compensate for skrink, the part should be
scaled instead of using the scale in the cavity function.
16) Don't use separate face colors unless necessary. Especially true of macros
that select many individual faces and color them. Individual faces are
difficult to change manually.
17) To color parts in the assembly, use part color instead of component
(instance) color except when there are multiple instances of a part in the assy.
18) Avoid surface features in preference of solid features when possible.
19) Use common sense when modeling threads, springs, or other complex geometry
that can be more efficiently represented another way.
20) Use of sketch relations rather than explicit dimensions (for example to
center a hole on a block, use a midpoint relation to a diagonal) when the
"design intent" allows.
21) Use incontext relations sparingly. Avoid circular incontext relations (A
references B, B refs back to A).
22) Fully defined sketches behave better than under defined, and defined using
relations which are relative to existing geometry are better than explicit
dimesions, especially when changes are expected.
23) Be careful to uniquely name each part. PDM software can help you do this.
Parts with the same name, even if in different directories will cause
"undesireable" results.
24) Split lines early in the feature tree can cause parent/child nightmares if
the sketch entities of the SL sketch are changed or the SL is deleted.
25) For plastic parts, the rule of thumb for order of operations should be
fillet1, draft, fillet2, shell, fillet3. Fillet1 is on an edge that is parallel
to the direction of pull, fillet2 is on an edge perpendicular to the direction
of pull with a radius larger than the shell thickness, and fillet3 has a radius
smaller than the shell thickness. There are, of course, many exceptions.
26) When revising a symetrical part where half was mirrored, suppress the mirrored half
before performing any modifications.
27) Use a many geometrical constraints as you can when fully constraining a profile. This
will greatly reduce the number of dimensions required and makes it easier to get desired
results when making adjustments.
28) When creating a complex part model I have found it helpful to create a master profile
and then convert entities on sections of the master profile to create additional profiles to
perform various operations.
29) When putting an assembly together that wil be used to create other assemblies later
think about how the mates will affect the assembly when the parts grow or shrink in size.
30) If you renamed a part in an assembly it is not necessary to delete the old part and the
new renamed part in the assembly. By right clicking on the part in the tree you can find
the option to replace a part with another part of a different name.
31) in order to rotate portions of a sketch in relationship to the origin and/or other
portions of a sketch you can use either constraining relationships and a dimension or a
circular repeat pattern.
32) Double click a mate distance in the assembly tree in order to display the dimension to
include it in an equation.
33) Use faces for mating relationships in an assenbly over edges and points when
possible. Faces will give you a more stable position for part.
34) You can use most AutoCAD commands in SolidWorks if you go under tools, add-ins,
while in a SolidWorks drawing and select the 2D emulator there.
35) When mating objects with little or no flat edges use reference planes for mating the
part to the assembly.
36) When applying profiles to edges to be swept, when positioning the profile get it as
close to the point where you want to place it before adding relations to nail the position
down.
37) When mating and the part mates to the wrong side or wrong direction, click the anti-
align to get it to mate the way you want it.
38) To have drawing views with suppressed parts you must specify a different
configuration to show the part(s) suppressed and unsuppressed and then import the
different named views into the drawing.
40) To use the middle button rotate option for 3 button mouses make sure in the mouse
settings in windows that the middle mouse button is set at Middle Button.
41)BOM's, when they become too long for the page size there is no way to resize them
easily, to breakup the BOM right click on the BOM and click on properties and click the
control tab. Then select the split table button, split to the right and give table height
(generally 210mm).
42)When using dual dimensions, you will want your English dimensions to be in
fractions, to get them the way you want them go under tools...options...document
properties. Make sure that the Dual Dimensions Display box is checked. Also then go to
the units branch of the tree and linear units box is set on inches. Then this happens other
boxes will become accessable. Check the fractions box underneath the unit box. Then
enter what you want the demoninator to be...8=1/8", 16=1/16", etc... Also make sure the
round to nearest fraction box is checked.
43) Instead of projecting views when in a 3-view drawing you can now highlight a view
in the drawing and by clicking on the dynamic rotate button it will open a dialog box
which will allow you to type in the degree of rotation on the part to get your other views.
44) A trick for tiling parts and drawings on you screen. By clicking on
tools...customize...keyboard. In the categories column click on Window. In the
Commands click on Tile Horizontally. You can assign the new keystroke to this
command say "T". Click on the assign button after your done. Now when you're in
Solidworks and you want to tile the different pages just hit the "t" key and this will now
do it saving you several mouse clicks.
45)To find out what mates, dependencies, etc... are associated with your features right
click on the top level assembly and click on view dependencies in the menu. This will
then organize all of your mates and other dependencies under which feature it is
associated with.
46) For our computers it is advisable that you should delete the contents in the
TEMPSWBackupDirectory and also in the TEMP folder out on your C drive at least
every other day. The size of these folders is usually over 100 megs and serve no purpose
other than a backup file of your latest changes on the parts you have done. Make this a
daily habit.
48) When sketching, if you don't want the geometry you are placing to be subject to the
inferencing snaps you can turn them off under sketch tools and uncheck the Automatic
Inferencing box.
49) SolidWorks will not allow swept profile intersections on angles other than 90
degrees. In order to get around this to achieve a more precise model representation of a
part you can extrude cuts followed by fillet operations to create the desired cross sections.
50) "Save as Copy" versus "Save As": To create a new part with no links to the prior
parts you will want to "Save As". Make sure to do this that you change the directory
where the part will be saved to, to be different than the part you are using. Also make sure
to change the name of the part. According to SolidWorks if this is not done, sometimes
the links will still be maintained wve nwhen you don't want them.
51) Design Tabels versus Configurations. There are now links between a design table and
configurations. So if you create a design table and then open the part and create another
configuration at the part level. The new configuration will not be seen in the design table.
To add configurations always add them in the design table.
52) To save all your options that you have set up on what toolbars and icons you have
showing follow these steps:
1)Start
soldiworks 2000
solidworks utilities
copy options wizard.
2) Pick out your user name and follow the wizard to finish.
53) When something in a drawing or part will not rebuild, even after making changes,
press CTRL-Q at the same time to force SolidWorks to rebuild everyhting in the model or
drawing.
54) To copy a part or assembly created by another person so as there are not links back to
the original parts/assemblies (i.e. when you change the new parts, you don't change the
old parts) follow these steps:
1) Start---Programs--SolidWorks 2000--SolidWorks Explorer
2) When the explorer is open go to File and browse to call up the part or assembly
3) With the part/assembly open, right click on the the part/assembly and click on
"copy"
4) Another screen comes up. Click on the "copy children" box. There should now
be two areas to browse where to place the parts and what to name them. Make sure both
places are pointing to the same location. In the "to:" field make sure you name your part
or assembly something different that what it was., while in the "folder:" field you save
these parts to a different location than where it is now.
5) Click "apply"
6) Open new part or assembly in SolidWorks.
