rocksolid perspective – jason raak

Just like what triggered my post last weekend “rocksolid tutorial: modeling a variable profile helix cut” I was recently asked a question by a member of my user group about how to simulate the stroke of a cylinder in SolidWorks.  So here we go, this is how I would simulate a simple cylinder stroke in SolidWorks.

As you can see in the above picture I have quickly assembled a bottom plate (green) that is housing a gas cylinder (yellow) in a pocket.  I also have a top plate (red) that is mated to the bottom plate with a distance mate called “open/close distance” which we will discuss later.  My gas spring was modeled with a simple single sketch profile revolve as you can see below.

By creating my gas spring as a revolve it is extremely easy for me to add a coincident mate between the top of the edge (which represents the end of the gas spring cylinder) and the bottom edge of the top plate.  You can see that I have both of those entities highlighted in red in the above picture.

Once you I added this relation you can see that the sketch of my gas spring is now fully defined.  You will notice that I also have added a driven dimension on the overall length of the gas spring which I can monitor to make sure that it does not exceed the limits of the stock spring.

Once I have done that you can exit your sketch and stop editing the part in your assembly.  Now you are ready to edit the mate that I mentioned earlier.  I have named this mate “open/close distance” so that I can quickly find which one I need to change.  By editing this mate you can simulate the top plate moving downward towards the bottom plate therefore compressing the gas spring cylinder.  You can see in the above picture that my distance “open” distance is 5.170in.  When I change this value to 4.170in., which is my closed distance (shown below) you can see that my cylinder compressed like I am wanting to see.

This is just a quick and easy way to simulate this cylinder compression.  As is with most things in SolidWorks, there are many ways to accomplish this exact thing.  If you prefer using an extruded boss/base cylinder you can use the “Up to Surface” option which will result in the same results.  If you have another favorite way to do this type of thing please feel free to share.

This week I was sent an email from a member of my user group with a modeling challenge.  They needed to model a helix cut that had different widths at the start point and end point.  I first thought that this could get pretty involved with different sketches and profiles but after playing with it for a few minutes I realized that it is actually quite simple to accomplish this.  Here are the steps I took to get this variable profile helix cut.

I started the model by creating a simple shaft with a chamfer on the top.  I then offset a new plane off of the top plane that I want to use as the beginning (or ending depending on which way you think) of the helix cut.  You can see these first couple steps in the above screenshot.

Next I created the 2 sketches that I want to use for my beginning profile (shown in red above) and my ending profile (shown in yellow above).

Then I created the helix that I want to follow by starting it on my helix start plane and telling it to do 1 revolution in the distance to the bottom of the shaft.  The helix I created is shown in blue in the above screen shot.

The next step is where I actually create the cut.  I used the “Lofted Cut” command.  For my 2 profiles I used the 2 sketches that I created earlier.  Now 1 thing to keep in mind when doing this is that we you select the sketches SolidWorks puts a green point at the closest end point of the sketch.  You will want to make sure that those end points are at the corresponding points on both sketches.  You can simply drag and drop the points to to the correct location if SolidWorks misinterprets where to put them.  Next, I used the helix that I created as the Centerline Parameters of my loft.  This allowed my loft to rotate around the part like I wanted.

Voila, it worked and I achieved the desired variable profile helix cut that I wanted.  If you have another way to accomplish this same profile please feel free to share.

A couple of years back one of the enhancements to SolidWorks was the thumb wheel that appears underneath the dimension in the modify box that appears as shown above.  If you are not familiar with this feature and just thought it was a cute and cuddly graphic that they added you need to know what this does first and foremost.  By simply clicking on the thumb wheel you can drag it either left or right to increase of decrease your dimension, pretty nifty huh?

Changing Your Increments

Now depending on what you use SolidWorks for you may want change the increments that the wheel changes your dimension.  Piece of cake!  All you need to do is go to Tools > Options > System Options > Spin Box Increments.  Here is where you get some different options.  There is 2 different length increments that you can preset, English units and Metric Units.  Then you have the ability to change Angle increments as well.  If you are working on more precise designs you may want to set these increments smaller but if you are working with wide open tolerances you may want these larger.  Totally up to you as long as your mom, dad, wife/husband, kids and the creepy neighbor down the street approve or your decision.

Changing on the Fly

You thought we were done already didn’t ya?  Not so fast!  There are always those times when you want to tighten or loosen up what you set your thumb wheel increments to.  Instead of having to go in each time and change these you can sort of kind of do this on the fly.  By holding down the Ctrl key while spinning the thumb wheel it will increase your set increments times 10.  So lets say you have your increments at 0.10in (as shown above), by holding down the Ctrl key your increments will now be 1.0in until you stop spinning and release the key.  Likewise, if you hold the Alt key while spinning it will decrease your set increments divided by 10.  So in the previous example your increments would be 0.01in.  Nice and simple!

Source of the Information

This is a tip & trick that I learned from Mark Biasotti at the West Michigan SolidWorks User Group meeting that was held on Tuesday, May 12.  This is the awesome kind of stuff that you learn at user group meetings and the best thing about it is that his presentation was on surfacing, but even if that topic is not your forte you can still pick up great tips and tricks like this one.  So if you are not an active or regular member of a user group in your area you need to become one.  If there is not a group in your area, let me know and I will get you the contact information of someone that can hopefully help you start one.

I have been accused in the past of being sort of any organizational freak.  I am one of those people that usually does not like stacks of papers on my desk and have more labeled hanging file folders than you can shake a dead squirrel at.  This is why I have become a huge fan of using folders in the FeatureTree to organize.  Folders can be quickly added inside your part and assembly files by RMB clicking multiple features, parts, or subassemblies and selecting “Add to New Folder”.  Why would you want to do this you might be asking?  Well, that is a perfectly legitimate question that I am hoping to answer for you in this post.

Why?

As I stated above the answer is simple, organize and clean.  When you are working on the 500+ feature part or that 750+ part assembly wouldn’t you want to keep your FeatureTree as short as possible so you can easily find features or parts as you go.  I am never a big fan of scrolling, then scrolling some more, then even scrolling some more to find that one feature that I needed to quickly modify.  By having folders you can shorten up that tree and eliminate all of that time wasting scrolling.

4 Quick & Simple Uses

Move Subassemblies – Move a solo or group of subassemblies inside your master assembly.  If you are like me and use subassemblies from time to time you might have noticed that it can be a pain to move that subassembly up or down your FeatureTree.  By adding it/them to a folder you can move the whole folder, then delete the folder and your FeatureTree will be organized like you are hoping for.  Tip – another way to accomplish this is by holding down ALT while dragging a subassembly to relocate.

Group Common Parts – Do you have a whole pile of nuts and bolts scattered in your FeatureTree or maybe a mole hill of springs and pins.  Well if you have more than 1 of the same component in your assembly FeatureTree I would highly suggest throwing all of the common items in a folder and label the folder whatever you please.  I usually create a folder with all the components I drag in from our Design Library because these are non editable, no drawing files that need to be in the design.

Group Common Features – Just like the common part use this is a nice and easy way to quickly group all of your chamfers, radii or even reference geometry into a folder so that you don’t have to stare at its boringness during your entire design process.

Move Multiple Features at the Same Time – You may have seen this warning before about dragging multiple features all at one time.

Well by dropping them all in a folder you can move all of these features at one time with out having to move each one individually.  Can you say…time saving!

Closing Remarks

This option gives me that warm and fuzzy feeling when I finished up a model because I know my FeatureTree is nice and orderly.  Well on second thought, maybe that feeling is the burrito I had for lunch.

So do you use folders and if you do how do you use them?  Please drop me a comment and share what your experiences are with folders.

UPDATE:  Thanks to Brian from CADFanatic for pointing out a misprint of mine.  To move a subassembly in the FeatureTree without dropping it into another subassembly you need to hold down ALT to drag NOT Ctrl.  Sorry for the mistake.