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.

The Answer to “Who is using 3D Mice?”

The results are in from my previously posted polls.  I have three results from two polls about who’s using 3D mice, and how they got them.  How did I get three results from 2 polls?

Well the first result of the polls is that I really dislike the polling site memedex.com.  I wish wp-polls would work, but it does not right now for my blog.  Oh well.

Ok, with regards to the second poll first, the question was “If you have a 3DConnexion 3D mouse, did you…?”

  • …buy it yourself (55 votes)
  • …get it through your company (49 votes)
  • …win it in a contest (14 votes)
  • …receive it as a gift from 3DConnexion (8 votes)
  • …steal it (3 votes)

So, it looks like most users either buy own 3d mouse, or their company bought it for them to use.  I am surprized at the number of people who have bought these devices for themselves.  I guess that says something about the usefulness of such devices.

Something that isn’t really a surprize, but worthy of mention is that 3 people actually admitted to stealing or otherwise obtaining one through some nefarious means.  I added this option to the poll almost as a joke, but I knew someone would come forward, so it was a legit option.  You 3 thieves!  ::shakes fist::  😉

“Do you use a 3D mouse with your 3D CAD application?”  The answers to this poll are skewed.  By a wide margin, responders stated they used 3d mice. This was kinda expected since the title of the article naturally drew in such users and likely precluded many of those not interested in 3D mice.  Regardless, here are the results.

  • Yes, everytime I use 3D CAD. (75 votes)
  • No, but I want to. (26 votes)
  • I have one, but I rarely use it, if at all. (21 votes)
  • No, and I don’t want to. (17 votes)
  • Yes, often or sometimes. (12 votes)
  • No, what’s a 3D mouse? (9 votes)

I think I know what the next poll will be.  I use my SpacePilot PRO with SolidWorks (and Google Earth).  With what applications are other people using their devices?

And the May Contest winner is…

The winner of the May Contest is Deepak Gupta! The contest was to see who could list the highest number of SolidWorks related forums not currently listed at Lorono’s SolidWorks Resources.  The contest itself generated over 70 comments, with about 65 or so submissions.  I am personally amazed by the total number of submissions. 

For his efforts, Deepak wins a CSWSP-FEA test.  From the SolidWorks website,

“The Certified SolidWorks Professional Simulation Specialist exam is designed to test an individual’s complete understanding of Simulation tools inside SolidWorks. Candidates who successfully pass this certification exam have demonstrated the ability to set up, run, and examine the results of various types of Simulation scenarios. They also have demonstrated the ability to interpret the various results available to them in SolidWorks Simulation.”

Best of luck to you, Deepak.  I’ll send you the info for taking your test by the end of the week.  I hope you pass with flying colors! 

Honorable mention goes to Frank Dijkstra.

The June Contest will be announced next week. Best of luck to everyone!