New in SolidWorks 2014: Slots in spades

This entry is part 10 of 13 in the series New in SOLIDWORKS 2014

A big leap forward for the Hole Wizard in SolidWorks 2014 is the support of slots as features!  I’ll say this another way.  You can now create slots with Hole Wizard!

When SolidWorks first announced that there was going to be support for slots many years ago, I was a tad bit disappointed when I found out how.  Slots were only available as sketch elements.  Although I did find this useful and it did streamline my workflows, I found it to be a step short.  I was still having to make slots as separate extrude-cut features.  Converting holes to slots and slots to holes still needed a rather lengthy workaround.

SolidWorks 2014 addresses this, and how!  Slots are now supported by the Hole Wizard in spades.

Slots slots slot

Slots with counterbores, slots with countersinks and slots with..umm, well, straight slots with no counter-anything.

Not just that, you can quickly switch between slots and holes, based on design needs for your particular phase of development.

Pre-slotPost slot

Holes become slots with a quick edit (and then back again, if you wish)


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.


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.


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.


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.

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.

SolidWorks 2009 is slated to introduce Slots functionality

At SolidWorks World 2008 (SWW8) we saw confirmation of a rumor.  SolidWorks 2009 would have the capability to add slot holes to parts.  This is a long sought after function that some would say has been missing along.  As demonstrated, the slot hole was not a special feature.  It was a sketch tool! Some may not initially like this, preferring slot holes to be their own discrete type of feature.  Others may prefer creating slots with a special sketch tool.

The SWW8 demonstration showed the presenter starting a sketch, picking the slot tool.  This allowed him to draw just a construction line with two LMB clicks.  The slot form automatically formed as though it was a capped offset from the initial construction line.  One more click set the sketch entities for the slot.  It appeared to be easy and painless.  I presume dimensioning of the slot within the sketch would be similar to current methods for similar sets of entities in the current version of SolidWorks.

The advantage to the slot function as a sketch tool is that user can actually create either an extrude or cut-extrude with the same tool.  So, not only are slot holes supported, but so is their opposite and positive counterpart.  As long as SolidWorks allows the user to dimension the slot hole on the drawing with the Hold Callout function, I do not have any major issues with this.  A mild criticism is that this method is a kin to how holes were made in the earliest SolidWorks versions, long before Hole Wizard, and presumably even before those “legacy holes”.  Perhaps this is just the first volley in a long series of improvements as we work our way to a Slot Wizard?  Maybe not.

However, some users might be expecting slot holes to be a feature of their own.  I cannot fully imagine how SolidWorks might accomplish this.  Maybe special one-off sketches are required, with sizes regulated with a Property Manager, similar to Hole Wizard holes.  Thinking of this, I can imagine that it would be nice to have some feature level control over slots so that they can be automatically sized when associated with a particular fastener within an assembly.

As far as dimensioning for slot holes on drawings, I did participate in early questionnaires regarding how this should be done.  I dutifully pulled my advice from ASME Y14.5M-1994, with special attention to Fig 1-35(b).  I also stated that I preferred centermarks to be at the center of slot by default (again referencing Fig 1-35(b)).  This will allow the quickest and simplest scheme to specify a slot hole.  This brings to mind a question.  If Hole Callout does callout slot holes this way, what will it do for extruded shapes that use a slot sketch?  There is no standard for this in ASME as far as I can tell, other than just directly dimensioning the feature.

There is one major point of concern.  How does this function translate into model assemblies?  Does SolidWorks 2009 quickly identify the slot hole center when smartmating a fastener at that location?  Right now, I always groan when I have to mate a screw to a slot because so much has to be done directly by me.  Update: something as simple as a temporary axis at the center of slot hole will be enough to address this issue, I believe.

One minor question of mine is how would slot sketch entities be handled within a sketch?  I think it would be best if they are recognized collectively as a slot, but can also be “exploded” into individual entities when other shapes based on the initial slot are desired.

I am looking forward to regularly using the new Slot functionality.  It promises to be a great timesaver that is well overdue.