SolidWorks Standards and Best modeling practices?

[SWUSER]

Hello SolidWorks Users! <br>
<br>
I would like to start a new topic on this message board that, hopefully, will be of some use to all of the SolidWorks users. <br>
<br>
There are many users out there who have discovered: <br>
- clever ways to create certain geometry in SolidWorks, <br>
- or best ways to create models, <br>
- features in a model, <br>
- put together assemblies, <br>
- ways to handle large assemblies, <br>
- and create detail drawings. <br>
<br>
Additionally, most of you have come up with company standards that maybe helpful to others when they want to write similar SolidWorks Standards for their own companies. <br>
<br>
The SolidWorks users do not share best practices and standards knowledge very well with others Users. I have written/collected over 30 of these best practices. I would like to add more to the list. I am sure most of SolidWorks Users have tips and techniques, best modeling practices, and proven standards that they have developed over the years, that they would like to share with other users. I would like to collect them and add them to the list that I have and Post them on here or email to the individuals that share their knowledge. <br>
<br>
Please post your post your replies on here or email them to me. Lets make this topic beneficial for all SolidWorks User. <br>
<br>
Thank You! <br>
<br>
<A HREF="mailto:Kiboeing@hotmail.com">Kiboeing@hotmail.com</A>

 

[wilfong]

Yes, I think this is a good idea. As a brand new SW user (just went to class last week) I am interested! Other people in my company are now going to class so we need to address this issue (we are all long time ACAD users).<br>Jim

 

Here are some best practices.&nbsp;&nbsp;I do hope people will add more to this! <br><br>Thanks <br><br>KIB<br><br>1)&nbsp;&nbsp;Use symmetry about part origin when possible.<br><br>2)&nbsp;&nbsp;Rename critical features to make them easy for other people to find.<br><br>3)&nbsp;&nbsp;Use a rational order of operations, expecially if other people may be using<br>your parts.&nbsp;&nbsp;Reasons for transgressing this rule would be to accomplish a<br>workaround that because of a bug or limitation cannot be done a better way.<br><br>4)&nbsp;&nbsp;Separate holes into different features to make suppressing them individually<br>possible.&nbsp;&nbsp;Don't create holes by making nested extrude sketches.<br><br>5)&nbsp;&nbsp;&quot;Multiple radius&quot; fillets promote poor design practice.&nbsp;&nbsp;Use &quot;constant<br>radius&quot; fillets where all fillets created by a single feature have the same<br>radius.<br><br>6)&nbsp;&nbsp;For mold and plastics design, to compensate for skrink, the part should be<br>scaled instead of using the scale in the cavity function.<br><br>7)&nbsp;&nbsp;Don't use separate face colors unless necessary.&nbsp;&nbsp;Especially true of macros<br>that select many individual faces and color them.&nbsp;&nbsp;Individual faces are<br>difficult to change manually.<br><br>8)&nbsp;&nbsp;To color parts in the assembly, use part color instead of component<br>(instance) color except when there are multiple instances of a part in the assy.<br><br>9)&nbsp;&nbsp;Avoid surface features in preference of solid features when possible.<br><br>10)&nbsp;&nbsp;Use common sense when modeling threads, springs, or other complex geometry<br>that can be more efficiently represented another way.<br><br>11)&nbsp;&nbsp;Use of sketch relations rather than explicit dimensions (for example to<br>center a hole on a block, use a midpoint relation to a diagonal) when the<br>&quot;design intent&quot; allows.<br><br>12)&nbsp;&nbsp;Use incontext relations sparingly.&nbsp;&nbsp;Avoid circular incontext relations (A<br>references B, B refs back to A).<br><br>13)&nbsp;&nbsp;Fully defined sketches behave better than under defined, and defined using<br>relations which are relative to existing geometry are better than explicit<br>dimesions, especially when changes are expected.<br><br>14)&nbsp;&nbsp;Be careful to uniquely name each part.&nbsp;&nbsp;PDM software can help you do this. <br>Parts with the same name, even if in different directories will cause<br>&quot;undesireable&quot; results.<br><br>15)&nbsp;&nbsp;Split lines early in the feature tree can cause parent/child nightmares if<br>the sketch entities of the SL sketch are changed or the SL is deleted.<br><br>16)&nbsp;&nbsp;For plastic parts, the rule of thumb for order of operations should be<br>fillet1, draft, fillet2, shell, fillet3.&nbsp;&nbsp;Fillet1 is on an edge that is parallel<br>to the direction of pull, fillet2 is on an edge perpendicular to the direction<br>of pull with a radius larger than the shell thickness, and fillet3 has a radius<br>smaller than the shell thickness.&nbsp;&nbsp;There are, of course, many exceptions.<br>

 

[mrcadd]

I have been a member of uor forum for maybe 5 minutes now - this looks good !

David Pennington

 

[BandH]

This sounds like a good idea - I've been using SolidWorks full time for 2 years now, and find it is a very good package.

One tip I would suggest is to make assemblies as &quot;stable&quot; as possible i.e. have enough mates applied to prevent accidental movement. If parts are not mated properly, when you insert a new part and then move it, there is a possibility of other parts moving as well.

If the assembly has to move, then I like to use a sketch to control the movement - for example, I've used a sketch to control the movement of a suspension assembly by only editing one angle. The parts in the assembly can be mated to the sketch lines in the normal way.

Hope this has been of some help to you.

Regards

 

[MikeDormanSDM]

To make my models clearer, I always begin drawing a part so that it naturally orients itself with the front, back, top... buttons. Doing so makes assembly much easier to mate.

Also, within assemblys it is possible to mate the planes of a part to the planes of an assembly. I always do this with the first part, instead of using the &quot;fix&quot; command. When the parts are lined up correctly with the assemblys planes, it is also much eaiser to use the functions like ruler and dimensioning, and also to postion holes on an assembly.

Good day!! [sig][/sig]

 

[dsi]

This is a great idea! I have been using and automating SolidWorks for almost two years now. Instead of posting them here, as a question, you should create a FAQ for this topic and point people there. [sig][/sig]

 

[gothic03]

Howdy all!
I've been using SW for a couple of years now, and my current employer has given me the reigns to develope a design standard as well. I've been working on it for several months now on &amp; off, tweaking &amp; revising. This thread has the potential to do a great many things for fellow SW users as well as myself, so I'd like to encourage everyone to reply. After all the only bad ideas are the ones left unspoken.

I've got a couple of things we're doing, and I was hoping for your suggestions for improvement or maybe some of our ideas may bring about other revelations.

1. We have separated our files(part, ass &amp; dwg) into seperate directories under our work orders on the network. This aids in finding files someone else has worked on, especially when you start to accumulate large numbers of files.

2. I created our standard title blocks with the company logo &amp; placed them on the network for everyones use. I've used custom properties for virtually all the title block info, so all you have to do is hit Alt+P then fill out all the information for the seperate items in one dialog. This eliminated the need for editing all the info seperately.

3. I created a standard part &amp; assembly templates to start new files with, and they include custom properties that are necessary to fill out our BOM template.

4. I created a template for each of our title blocks as well. When I go File-New I get a list of my part, assembly &amp; title block templates to choose from, and since they're on our network we're all using the same thing.

5. We all use the same background colors for our files, because if someone uses white on black &amp; someone else uses black on white, when they open each others documents they would have to do several color changes right off the bat to even see anything. Not a real big deal, but confusing to newer users. We also standardized the color schemes for sketches to allow us to know quickly whether a line is fully defined or under defined.

6. We design various automation, end of arm tooling, fixtures, but mostly plastic injection molds, and we're trying to standardize how we do our part splits. Maybe someone may offer some advice on this. Currently we:
place part in block of material, cavity it out, derive cavity, core, lifters, etc. from this &quot;initial split&quot;. Then we form an assembly to mate all these parts back into to double check shut-offs, etc. We start getting very slow
files about 1/2- 3/4 of the way through the design with all the in context features. The assemblies start getting very slow &amp; we can't figure out why, they really don't get all that large. 150-200 parts generally. Ideas?

7. We also rename our critical features to aid in downstream interpretation of our files. This little time up front can save head aches later.

I'll get going for now- digest some of this &amp; give me your opinions, ideas, or maybe I may have even given you some new perspectives. I'll add more to this later. Take Care.

Kevin Morris
Design Engineer
Techniplas, Inc.
Ankeny, IA 50021
kmorris@techniplas.com

 

[swertel]

We have had SWX for about a year now, but are finally to the point of &quot;practicing&quot; with a few of our product lines to get everyone proficient enough at SWX to say &quot;This is how we're going to do it.&quot; One concept we have in mind is using a master model. Our product line consists of core features and typically only dimensions change on those features. So, we bring in a master model with all (most) of the features defined and we modify dimensions. That way the FeatureTree always looks the same (named features) and the design table and other embedded information also has the same format. In addition, we use CAMWorks which embeds its machining information into the part file. Our master model contains this info, too, so our CNC programmer does not have to completely rebuild code for every new part.

I'll be happy to share our templates with anyone who would like to see how we use custom properties to fill title block info, but not a master model (for obvious proprietary reasons).

Scott Wertel
Design Engineer
Interface, Inc.
Scottsdale, AZ 85260
scottw@interfaceforce.com

 

[dwilson]

There are many places to get information on the best practices and tips/tricks. Below is a link to a SW solution partner that publishes PDF files containing all kinds of information. This is where I started when I started an inter-company user group.

http://www.triaxialdesign.com/tip_tricks.html

Dave Wilson

 

[SJ]

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 &quot;Edit Sketch Plane&quot;
3) Dialog box comes up, select plane you want sketch to switch to, and apply

2) &quot;ESC&quot; 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 &quot;Select Other&quot; 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 &quot;Annotations&quot;
and highlight &quot;Hide all Feature Dimensions&quot;

5)With multiple drawings up, to switch between them without minimizing and
maximizing press &quot;Ctrl Tab&quot;, 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) &quot;Multiple radius&quot; fillets promote poor design practice. Use &quot;constant
radius&quot; 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
&quot;design intent&quot; 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
&quot;undesireable&quot; 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&quot;, 16=1/16&quot;, 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 &quot;T&quot;. 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 &quot;t&quot; 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) &quot;Save as Copy&quot; versus &quot;Save As&quot;: To create a new part with no links to the prior
parts you will want to &quot;Save As&quot;. 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
&quot;copy&quot;
4) Another screen comes up. Click on the &quot;copy children&quot; 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 &quot;to:&quot; field make sure you name your part
or assembly something different that what it was., while in the &quot;folder:&quot; field you save
these parts to a different location than where it is now.
5) Click &quot;apply&quot;
6) Open new part or assembly in SolidWorks.

 

[SJ]

Here's my two cents. some of the tips are missing since they only apply to my company.

1) To switch part creation plane from one to another:
1) Select the boss-extrude sketch
2) Right click and highlight &quot;Edit Sketch Plane&quot;
3) Dialog box comes up, select plane you want sketch to switch to, and apply

2) &quot;ESC&quot; 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 &quot;Select Other&quot; 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 &quot;Annotations&quot;
and highlight &quot;Hide all Feature Dimensions&quot;

5)With multiple drawings up, to switch between them without minimizing and
maximizing press &quot;Ctrl Tab&quot;, 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) &quot;Multiple radius&quot; fillets promote poor design practice. Use &quot;constant
radius&quot; 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
&quot;design intent&quot; 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
&quot;undesireable&quot; 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 assembly 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&quot;, 16=1/16&quot;, 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 &quot;T&quot;. 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 &quot;t&quot; 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) &quot;Save as Copy&quot; versus &quot;Save As&quot;: To create a new part with no links to the prior
parts you will want to &quot;Save As&quot;. 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
&quot;copy&quot;
4) Another screen comes up. Click on the &quot;copy children&quot; 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 &quot;to:&quot; field make sure you name your part
or assembly something different that what it was., while in the &quot;folder:&quot; field you save
these parts to a different location than where it is now.
5) Click &quot;apply&quot;
6) Open new part or assembly in SolidWorks.

 

[MadMango]

It's also a good practice to mates parts in an assembly with a Distance of zero. If you are using exploded models in drawings and other things, it's much easier to manipulate the assemby if all the mates are Distance rather than Coincident.

Another practice would be to create a Standard Parts Library on your server that is accessable to all SW users. If one person has already spent the time to model an off-the-shelf part, there is no need for another to duplicate the work. This goes for standard fixtures and other things that may be unique to your company.

 

[SBaugh]

This is a wonderful idea. These posting should be posted at the comp.cad.solidworks forum also.

Well, I have read over the entire list of standards. I have to say that most all of them are good and informative. But I would (if none of you mine) like to expand and possibly enhance a couple of them. Maybe it will help and may not. Please don't take offense to this.

Here it goes!

SJ wrote:
<snip>
33) Use faces for mating relationships in an assembly over edges and points when possible. Faces will give you a more stable position for part.

You are correct faces are better to mate to than edges and points. But the face is just as unstable. Planes of a particular part are the best. If you come to face of part(A) to mate too, open that part(A), make a new plane offset at a distance then mate the other part(B) to it.

<snip>
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.

The TEMPSWBackupDirectory is another way of slowing down performance. If you turn off this feature you will see a performance improvement. The problem with turning it off is that of course you will not be getting a auto backup every X amount of changes. So the user must learn to save often. I do this, and I have lost an hour or less of work do to a crash. But the performance improvement was worth it.

<snip>
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

Some added features using Design tables:
Assembly Design tables:
$Configuration@Filename<1>
$STATE@Filename<1>
For a listing go to SW help file.

Now for my .02 worth,

1) When doing a large assemblies, first thing that I suggest is to offset planes to use for mating. These planes need to be throughly, and completely thoughtout. This idea works great when you are incontexting the models (incontext the models only to the planes of the assembly and use them sparingly). Instead of controlling the parts and or distance mates, you can control the planes of the assembly. This helps in keeping the in-contexted relationships to a minimum, along with keeping cicular in-contexting out of the loop.

Thanks to Stan Sweet at the SW World Conference this year, for his presentation. It has helped me, get a better handle on my automation programs without the use of VB. Just an embedded Excel file in my models.

2) Maintaining Incontexted References - Special thanks to Per O. Hoel for his responds on this issue.

The issue is not the renaming of the file folder. The &quot;problem&quot; arises when the name of the assembly itself is changed.

To get around this, you need to follow these steps:

1. Create the new directory folder(s).

2. Open the assembly with the in-context relationships. MAKE SURE that ALL the parts are RESOLVED!

3. Save the assembly to a new file name (Save as COPY) to the new directory.

4. When the message comes up to inform you that there are in-context features that will not update in the new assembly, hit Cancel, uncheck the 'Save as Copy' option, and click References.

5. In the References dialog box you should select all of the parts listed that you want to be copied to the new directory. (Giving them new names is optional.) The Select ALL button is handy and then you can unselect certain
ones, if desired.

6. Once the files are selected, click the New Folder 'Browse' button. You should see your desired directory tree pointing to the folder you specified as the destination for the renamed assembly file. If not, or if you want any part to be copied elsewhere, just navigate to the proper folder (which must already exist). The easiest thing is to have all the parts go to the same folder as the assembly will.

7. When you're ready, click OK and then click 'save' in the Save As dialog box.

At this point you should see the open assembly adopt the new name and, if you check 'File/Find References', the active parts will be the copies in the newly specified directory. All the in-context references will be intact!

A helpful way to see how this works is to have an instance of Windows Explorer open with the directory displayed. Start with it empty and experiment with a small in-context assembly to watch the &quot;dynamics&quot;.

Per O. Hoel

I hope this has helped some of you,;-) Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com