Category: Part

Drill and Tap (~Part 3)

This entry is part 4 of 4 in the series Hole Callouts

I previously discussed threaded hole callouts in the context of SolidWorks and its calloutformat.txt files (Part 1 and Part 2). As mentioned before, there is a tendency for some to callout threaded holes with too much information. Often, the thread callouts include the drill size. As argued before, including the drill size usually over-defines the threaded hole because the specifications of the thread itself identify the drill size. It also attempts to specify manufacturing processes, which is not allowed by ASME Y14.5M-1994. In fact, including the drill size within a thread callout may actually provide incorrect specification in many cases.

This is particularly true in the case of threads that are in blind holes. These are usually made with forming taps (roll taps). The diameter of the drilled hole for a roll tapped thread is bigger than it is for a cut thread. For example, for a 10-32 roll tap, the drill size is .1762, while a 10-32 cut thread drill size is .159. Once formed or cut, the specification for the ID of the thread is .156 to .164.

On drawings where customary units (inch) are used, the number of decimals places in the dimension usually determines the tolerance for that dimension. Stating a drill size as a decimal dimension applies the standard drawing tolerances to that dimension unless some general note is added.  This means that the tolerance for the drill callout likely differs with that required by the thread.  So, if the drill size is called out, drawing may be providing the wrong information to the machine shop.

Hole Callouts: Why is THRU sometimes THRU ALL?

This entry is part 3 of 4 in the series Hole Callouts

Question: On a drawing, when adding a callout to a simple through hole or thread, SOLIDWORKS will sometimes add “THRU” and other times add “THRU ALL”.  Why does SolidWorks sometimes add “THRU ALL” in such cases, even though the hole is obviously just “THRU”  (“THRU ALL” being through multiple features and “THRU” being through just one feature.)

Two words: Design Intent.  SOLIDWORKS has powerful modelling tools that allow the user to establish design intent.  In the case of through holes and threads, this design intent is created by the user’s choice on how to make that hole through (its End Condition).

Notice, if a hole is added to a model where the end condition is blind, but the depth of that blind hole cuts through the part, the hole callout on the drawing will show stated depth and not the fact that the hole is through.  Here, the design intent is that the hole shall be cut to a particular depth regardless of the fact that the hole ends up being through the part.

By instinct, many of us pick “Through All” as our end condition for a hole.  However, SOLIDWORKS interprets this as the user’s design intent to make the hole through every feature, so the drawing’s hole callout is “THRU ALL” even though there is only one feature being drilled through.  To capture design intent of “THRU”, the end condition of the hole must be “Up to Next”. This tells SOLIDWORKS the design intent is that hole is only through the immediate feature regardless of how many features it may intercept.

For threads, both end conditions may be set to “Up to Next” for the design intent to be fully captured so that both bore and thread are called-out as “THRU” on the drawing.  A side note, thread callouts may still show depth, even if “Up to Next” is selected.  Be mindful of this.

If drawings already exist with non-modified hole callouts, simply updating the model will usually update the drawing callouts.

Control Root Size of Drafted Rib on Curved Surface

*This article makes some inaccurate statements regarding the capability of SolidWorks.  Please see the correction article for details.  Inaccurate statements have been crossed out.  The methodology described in this article should be referenced as an example of bad practice that should only be employed if traditional methods fail.  Edits to this article appear in this color.*
*Additional comment: this article does demonstration a good method for getting a line along a curved surface into a sketch. *

Good mold design means that one must take care to control the root width of a rib.  How does one do this if the rib is based on a curved (non-prismatic) surface? 

SolidWorks has many powerful features for making injection molding parts.  It has both rib and draft features.  Unfortunately, these two features together have one important limitation.  When applying a draft to a rib based on a curved surface, SolidWorks does not allow the user to hold the root width of that rib.  SolidWorks requires a prismatic surface to use as a neutral plane from which to start a draft.  This means in this case, the draft can only be started from the top of the rib, not its root.  If one wishes to hold the rib root constant along a curved surface, one cannot use the rib or the draft features.

SolidWorks does have an arsenal of other features and tools to allow one to build an alternative strategy to workaround this limitation.  

Basic shelled part with curved surface

This first figure shows a fairly simply shelled injection molded part with a complex curved surface.  To make drafted ribs using this method, first create an axis that can be used as an directional guide. You can choose to use features on the part itself for this purpose, instead. I prefer to create a special sketch at the location where I plan to add a boss.  Regardless of the method used, the directional guide should be parallel to the direction planned for the ribs.

 Setup Sketch for Directional Guide

The second step is to start a new sketch above the curved surface.  In that sketch, draw the outline of the rib.

Sketch outline of ribs

If there is a series of ribs needed in one direction, try creating a sketch pattern the other instances.  Make sure to turn sketch entities of the other instances into construction lines.

Project outline using Split Line

Use Split Line to project that outline onto the curved surface.  Split Line will only project one contour per sketch.  This is why it is important to turn all other instances of the rib into construction lines.  Having those other instances pre-drawn will save time when making the other ribs (covered in Part 2 of this article). 

Next, start a 3DSketch.  Use Convert Entitles to bring the Split Line curves into the sketch.  Drag the end points of the curves so they are coincident (on the surface) of the outside surface of the outer walls, or some othe appropriate location.  Then, close the contour by drawing lines to connect the curves at each end. 

Convert split line edges in 3DSketch

Extrude this sketch.  Use the previously drawn axis from the first sketch as the direction.  Use the top surface of the cavity (or whatever is appropriate) as up-to-surface entity.  Turn on Draft and specify the desired angle.  Here’s the funny part.  Be sure to extrude a small amount (smaller than the wall thickness of the part) in the other direction without draft.   If this isn’t done, a zero-point error will pop up preventing the completion of this step.

Use previous setup to set extrude of 3DSketch

The end result will be a drafted rib with a controlled root width.

Final result

Part 2 of this article will detail how to create repeated and crossing ribs using this same technique.  Again, please note this is not a best practice method.  See the correction article for details.

ctopher’s SolidWorks Material Database

*New database is now available.  Links in this post have been updated.  See new post here.*

The new ctopher’s Material Database (offsite link) is here! The long anticipated update of my material database.

The new database version 041008 has been updated with more materials.

Because of conflicts with some of the materials between SolidWorks 2008 and older versions, we created two versions. One version is for 2007 and older and the other is for 2008 and newer. Both are included in the same file.

Also added is a text file with instructions.

Thank you to Matt and others for your help and contributions.

Chris (ctopher)

Download page: ctopher’s Material Database (onsite link)

User Interfacing with SolidWorks (Make it faster, stronger, better)

Setting up one’s computer for using SolidWorks on a regular basis is a matter of personal preference in the extreme.  There is almost literally as many ways to set up a SolidWorks station as there are SolidWorks users.  SolidWorks provides many methods for user interface, including toolbars, peripherals, shortcuts keystrokes, menus, command manager and other assorted on-screen functions.  The most important element is the human in the real world using SolidWorks in the electronic realm.  The following is just some of my thoughts about things that can be done to make interfacing with SolidWorks easier.

Monitors

For me, I have found that two monitors works well.  I set up one monitor as my primary where I run SolidWorks and other high-end software.  I use the second monitor for reference and interfacing, to run such programs as Adobe Acrobat (PDF), PLM/ERP software, Internet, MS Office applications, commonly accesses desktop icons for these and other links of various type, etc.  I also place less frequently accessed SoildWorks toolbars on the second monitor.  Additionally, I place my SolidWorks command manager just on the edge of the second monitor where it is close enough for quick access, but removed from the main screen.  This opens up space for my model view pane.  It should be noted that I’m currently using SW 2007.  Moving the command manager is currently not possible on SW 2008, from what I understand.  I would like the ability to move the FeatureManager pane from the primary monitor as well.  I hope this is a feature that will be added in SW 2009 or 2010.  The goal for me is to have as much space as possible on my primary monitor dedicated to the view pane.

Also, I now recommend new widescreen flat LCD monitors of the 24″ variety or bigger.  The prices have fallen drastically, while the quality has improved radically.

Mouse

I have found that a lot of people are perfectly happy with very low movement settings on their mice.  This I cannot understand.  It amuses me that people will drag a mouse halfway across their desk surface just to have access to a corner of their Windows desktop.  They move their mouse 8″ just to click a toolbar icon, and them move their mouse another 8″ to get back to were they where.  This is a bad time waster.  It is also horrendous ergonomics, for which they will ultimately pay the price.

A mouse should be set to as sensitive a setting as needed to give the cursor arrow access to all portions of your monitor(s) within a very slight movement.  I have my mouse set so that I can access any point on my primary monitor within a 2″ diameter of movement using a medium threshold.  The threshold is the speed one moves their mouse to trigger faster movement of the cursor arrow.  More detailed local movement of the mouse should also be as sensitive as possible.

This allows the user to control their entire desktop with very little movement.  It increases speed of operation.  It is also more ergonomic, being better for a person’s long term arm, wrist and hand health.

Shortcuts

To reduce the need to move the mouse around even more, use a lot of single stroke shortcut keystrokes.  A lot of people may not like shortcuts for various reasons.  I believe one of the most common reasons is that they are too hard to remember.  However, they are worth remembering.  The time savings from using shortcuts verses moving the cursor arrow around is tremendous.  With the right sort of shortcuts set up, you can be working on one particular portion of your model and access several functions without having to move your cursor arrow back and forth from the toolbar back to your operating area.  You can be in a sketch, switching from line to dimension to circle to trim, all without having to move your cursor arrow off of the view pane.  This allows for much greater efficiency.

To make it easier to remember shortcut keystrokes, only add one or two at a time.  When familar with those, as a couple more based on what you use the most.  This allows you to learn/remember a couple at a time instead of a bunch all at once.

Of course, programming functions into the mouse itself will save even further movement of both your hands.  This usually requires setting up shortcut keystrokes in SolidWorks that are then mapped to the peripheral.  In this case, use very complex shortcuts such as CTRL-SHFT-F1.  It doesn’t matter how complex because it’s still just a push of a button on your peripheral.  Save the single stroke shortcut keys for other functions.

Strategy for Good Interfacing

A way of looking at interfacing with CAD software (particularly SolidWorks) is to think of functions in terms of how often you use them.  The more often one uses a function, the easier and quicker that function should be accessible.  One methodology is to work in the following way.  The top 5% of functions used should be accessible with very little movement.  If possible, they should be mapped to buttons on your mouse or other peripheral.  The next 15% of functions should mapped to single stroke shortcut keystrokes.  The next 25% of functions should be accessed through actual clicking of on-screen icons.  Any remainder functions should be accessible through the pulldown menu scheme.

Also, if you find yourself using a series of functions routinely, then create a macro that accomplishes those tasks.  Map that macro to a single or multistroke shortcut.  Always be mindful of repetitive tasks and the ways they can be simplified to save time and improve ergonomics.

Knowing how to implement this strategy doesn’t come over night.  It comes from working with SolidWorks over time.  As you work with the software and pay attention to your own actions, you will become aware of what can be done to improve your efficiency.  For me, if I repeat the same action over and over, I work to reduce the number of the steps it takes to perform that action until I get it to a point where it doesn’t bother me anymore.  Use whatever means necessary to this end.

Jumping Toolbars, Cadman! (Toolbar changes not saved)

With SolidWorks 2007 and prior, most commands are available through on-screen toolbars.  These toolbars are highly adjustable, both in content and placement.  Sometimes, their adjustability in placement can cause issues that may make it seem as though SolidWorks isn’t saving toolbar placements.  In my experience, SolidWorks does a good job at saving placements of toolbars.  The issue many have with saving toolbar placement is often related to the fact that SolidWorks allows the same toolbars to be placed in different locations for each document type (drawing, model and model assembly).

It should be noted that some people do experience a real problem with toolbar placements not being saved.  This problem is caused by a corrupt install or registry.  To correct this issue, use regedit.exe to rename/delete the SW registry key (HKEY_CURRENT_USER\Software\Solidworks).  This allows SolidWorks to establish a new registry key, and hopefully eliminate the corrupt information.  (Note: this will clear all Solidworks settings, so use this method with caution.)

But, before that method is attempted, try this less drastic method first.  As stated above, sometimes the issue is caused because different document types are using the same toolbar, but that toolbar is in different locations for each.  This causes them move around when switching between document types.  As they move around, they push other toolbars around too.  Each time this happens, they can cause toolbars to shift into even more different locations.  The solution is to have a drawing, model and assembly all open at the same time, then switch back and forth between them to see what jumps around. Adjust locations of the toolbars with each document type active.  Switch back and forth from that document type to the other types.  Do this for each of the three document types.  Keep doing this until all toolbar locations are stable, no matter which document type is open, and to which document type is switched.

Then here’s the most important part: exit SolidWorks normally.  It is the exiting of SolidWorks that saves the toolbar placements. The process can take about 5 to 30 minutes.

A side note, if SolidWorks crashes at any time after toolbars are changed, but before exiting normally, any changes to the toolbars will be lost!  This is important to note, it is it a third reason why toolbar changes aren’t saved.