And the June SW Legion Contest winner is… (Part 2)

There are two winners for the June SW Legion Contest.  The official winner (Sandeep Pawar) and the unofficial winner (per the unstated and unofficial though originally intended rules) is Arash Erfanian.   Three individuals produced verifiable scalene ellipsoids with only three elements.  One individual used two sketches and one feature (3 elements total).  Two other individuals used one sketch and two features (also 3 elements total).  These made cleaver use of the scale feature.  After a suprizingly quick game of email roshambo, Arash came out on top, earning himself a CSWSP-FEA test.  Congrats to Arash.  He knows his scalene ellipsoids, and he knows how to play a mean game of roshambo.

As mentioned before, I received 11 submissions.  One submission was of a model that only had one 3D sketch and one feature (2 elements).  However, I was not able to confirm its scaleneness.  The solution was cleaver though; leave it to Matt Lombard to come up with such a simple approximation.  One of the other submissions was a surface model (not solid).  Unfortunately, it had more elements than the solid model submissions.

I don’t have access to the submissions at this moment.  When I do, I will go into further details about how everyone accomplished the goal.  I am not amazed by the variety of submissions.   I was surprizes at some of the methods employed.

And the June SW Legion Contest winner is… (Part 1)

The June SW Legion Contest asked the brave ones among us to provide the very simplest ellipsoid within Solidworks.  It turned out that the rules where a little too general.  In my excitement to announce this contest, I failed to specify that I was looking for scalene ellipsoids, not just any old sphere.  I also left off the detail that I wanted a fully defined solid model.

Due to this oversight, I will be awarding two CSWP tests this month.  One test will go to the person that technically fulfilled the initial requirements.  The second test will be awarded to the person that produced the simplest scalene ellipsoid.

June SW Legion Contest has received eleven entries from ten individuals.  A couple of entries were just for fun.  One was a PDF of a model created in AutoCAD, and the other was a simple sphere submitted by a fellow blogger (who himself is giving away CSWPs, so does not need another one from me).  Technically, his entry would’ve tied with the other entry that used the same method to create a Prolate spheroid.

The easiest way to make a sphere or similar object in SolidWorks is to have a single sketch of an arc that is then revolved.  We have one serious entry that used this method by Sandeep Pawar.  He has requested the CSWP test.  Best of luck, Sandeep, and congratulations!

I have further review to undertake in order to declare a victor for the search for the simplest scalene ellipsoid SolidWorks model among the entries.  I have four very compelling entries which I’m currently looking over.  More details to come.

Different ways to Mate with a SLOT -1

Now we have finished and learned the techniques of making a SLOT, the second question comes up in the mind is “How to Mate with a SLOT”. Again there can be several ways to achieve this and one may adopt the method which he/she finds easy and quick to use. In this chapter let’s discuss about various simple ways of mating with a SLOT.

To use these methods you need a simple plate with a Slot of any size, a cylindrical, rectangular or square part with diameter/width equal to or less than slot width. In this chapter I’m going to use the cylindrical part (pin). I will be covering another discussion on same topic with a square part too.

Start you assembly with the plate inserted as the base part and fixed. You can also use mating techniques to position your plate. Now insert you pin which you want to mate with the slot.

MS1

Method 1: With your assembly opened and both the part inserted, select the back face of the plate and bottom face of the pin. Add a coincident mate between them. You can select front and top faces too. This is to set the initial position. Now show on the temporary axis (View > Temporary axis) to display the temporary axis of the pin. Select the side face of the plate and the temporary axis of the pin and give a distance mate. Repeat this with the bottom face. Your pin is now in to the required position.

MS4

Method 2: Using the same technique as described in method 1, use the planes instead of the temporary axis of pin to give distance mates with the side and bottom faces of the plate. Your planes may vary from the one shown in the picture.

The difference in the above two methods is that in Method 1 the part is not fully define and its free to revolve on its axis whereas in Method 2, the part gets fully defined.

Method 3: This is a combination of above 2 methods. Add a distance mate using the side face of the plate with the corresponding plane of the pin. Now show up the temporary axis if they are not on. Select either of the temporary axes of the slot and corresponding plane of the pin. Add a coincident mate.

Method 4: If your slot width and diameter of the pin and equal then you can use this method. Add a tangent mate between the side face of the slot and the cylindrical face of the second part. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane/temporary axis of the pin.

or

Method 5: In this method, RMB on the edge of the plate and select “Midpoint”. Then select the corresponding plane of the pin and add a coincident mate. Then add a distance mate with the bottom/side face depending upon the location of your slot with the corresponding plane of the pin.

Method 6: This is tricky method and I prefer to use this method most of the time. Open the plate and edit the slot sketch. Add these two construction lines to your slot sketch. Now in assembly, select to show the slot sketch. Use the planes of the pin and mate them with the corresponding construction line

 

 

These are few of the methods which I use for mating with a slot. I would be interesting to hear if you more methods or any other method that you use for mating with the slot.

June SW Legion Contest: Create an Ellipsoid model

The June SW Legion Contest is a different kind of challenge!  The task is to submit the simplest SolidWorks model of an ellipsoid possible.  The person with the least combined number of features and sketches wins.  Use of equations is highly encouraged. 

The submitter must be the author of the file they submit. 

Contestants may email their entry to me at my email address by the end of July 6, 2009 PDT.

Ellipsoid

The prize is one CSWP test of your choice (CSWA, CSWP, CSWP Sheetmetal, CSWSP FEA, etc).   

Past winners of the Legion Contest are eligible.  In the event of a tie, tie breaker will be in the form of email roshambo.

Best of luck to everyone!

Dimensioning of Slots in SOLIDWORKS for ASME Y14.5

This entry is part 4 of 8 in the series Dimensions and Tolerances

Ever since the additions of the slot sketch tool for 2009 and the Hole Wizard Slot for 2014, SOLIDWORKS almost seems like a whole new software for the those who design machined parts.  Adding these tools were long overdue.  Additionally, SOLIDWORKS supports the standard methods for dimensioning slots when they are created by using these tools.

ASME Y14.5M-1994 paragraph 1.8.10 and figure 1-35 provide three methods for the dimensioning of slots, with no stipulation regarding which is preferred for particular scenarios.   (Note: all three methods require the insertion of a non-dimensioned “2X R” note pointing at one of the slot’s end radii.)

In one fashion or another, SOLIDWORKS supports all three methods, though it does have a default for both simple slots and arc slots.  For brevity, this article will only cover simple slots.

The first slot dimensioning method (a) provides the width and the distance between the end radii center points.

Dimensioning Method (a)

Method (a)

The second method (b) is the easiest and simplest to dimension.  Simply state width and overall length, and use an arrow to point to the slot’s object line.  Though originally reserved for punching operations, ASME Y14.5M-1994 (and later versions) allows for the use of this method on any simple slot.  When using Hole Callout to dimension a slot in SOLIDWORKS 2009 or later, this is the type of dimension that is inserted.

Dimensioning Method (b)

Method (b)

The third method (c)  provides the width and overall length of the slot in linear dimensions.  This method is preferred if the slot has positional tolerances that use the boundary method (see ASME Y14.5M-1994 figure 5-47).

Dimensioning Method (c)

Method (c)

For all of the above methods, add the “2X R” separately by using Smart Dimension tool.

Side note: of the three choices, the ASME board almost left out (a) and (b).  The original release draft of ASME Y14.5M-(1994) only shows method (c) in figure 1-35.

Using Empty Views (Part 2: How to use them)

My articles on Empty Views in SolidWorks have been long in coming.  This is not due to the topic being complex or anything.  It’s just taken me that long to get around to this series.  (There’s been a lot of other stuff to talk about in the meantime, such as SolidWorks World 2009, something called a 3D mouse, and rants about this or that.) The Part 1 article in this series discussed how to make, place and size Empty Views.  Part 2 now discusses how to use them once they are created.

Use Empty Views as quick Zoom to selection locations

OK, let’s say that one empty view each represents the title block, revision block and drawing notes.  How does one quickly move about the drawing to view these areas?  There are several methods available in SolidWorks.  The following method is likely less common, but is perhaps quicker can more common methods.

First, assign a shortcut to Zoom to selection function.  Zoom to selection is found under View pulldown>Modify>Zoom to selection.

Zoom to selection location

To add the shortcut (for much quicker access to this function), goto Tools pulldown>Customize…>Keyboard tab> and then search for “zoom to selection”.  From there, simply add a keystroke as the shortcut for Zoom to selection and choose OK to save.

Now here is how to use this shortcut with Empty Views.  With the drawing open and with no views selected, look over in the FeatureManager.  Select any one of the Empty Views (or any view for that matter).

FeatureManager display of views

As this point, simply hit your shortcut keystroke for Zoom to selection.  The viewport will immediately zoom to the area identified by the Empty View.

Zoom to selection of empty view

Choose another view from the FeatureManager and hit your shortcut for Zoom to section again.  Each time, the viewport will immediately zoom to the area defined by the selected view.

Using Empty Views for PDF bookmarking

As an added bonus, any views created on the drawing (including Empty Views) will become bookmarks if you save that drawing as a PDF.  This adds greatly to the navigability of PDF files for everyone who uses them.  Within PDF Reader, the bookmarks will appear to the left (similar to the FeatureManager in SolidWorks).  Simply LMB click on the desired view, and PDF Reader will jump to that location.

There are some pitfalls with saving a drawing as PDF, so if your company is experiencing those, then it is not recommended that drawings be saved as PDF.  In those cases, print to PDF works better.  Unfortunately, bookmarks are not created when printing a drawing to PDF.

Conclusion

The one thing that frustrates me about SolidWorks Empty Views is that SolidWorks Corp reduced their functionality (as discussed in Part 2).  However, with a simple hack, they can be used as drawing bookmarks, to contain drawing notes,  and to add functionality to PDF files.  Additionally, they are always useful for containing sketches, as noted in Part 1 of this series.