Avoid Obvious Tessellation during your 3D Printing Jobs SolidWorks file for FDM Printing

How did your file get from this:
 To this?  

Did you ever stop to check if the STL file you sent to your Stratasys printer looked like this?

The solution to this problem is simple… check the STL Save Options:

Set the Angle tolerance to 3 to control the smaller detail tessellation.

Never again will your tessellation be as obvious as this:  But now you can look forward to smooth parts like this:

 This SolidWorks Tutorial With  Sketching

Don’t Double-Click to Select a Sketch Plane
If you double-click on a plane it will be deselected, although the plane will stay highlighted. If you have not properly selected a sketch plane, SolidWorks will not begin sketching when you click the Insert Sketch icon. As a windows-native system, Solidworks closely follows the “Object-then-Action” workflow, so pre-selection of geometry is key to allowing the User Interface to anticipate what you want to do next.
On a related note, we recommend that you do not use the INSERT – SKETCH in SolidWorks   icon for editing an existing sketch, but instead use it only for creating new sketches. Although the documentation suggests that this icon can both Create and Edit, the edit mode will only work if you have carefully pre-selected the desired sketch to edit. It is common for novice users to forget the pre-selection, and thus they end up working on a new sketch on the same plane, but are ‘insulated’ from the lines they had hoped to edit. Since Solidworks 2008 now offers context-sensitive pop-ups, including the EDIT SKETCH icon, on the selection of any sketch entity,, the old method of editing by re-selecting the INSERT SKETCH icon is actually extra clicks and should be disregarded.

Avoiding Accidental References in SolidWorks 
The Solidworks sketcher saves time and assists the new user by automatically capturing many different relations in a sketch automatically. However, as a user gains experience, and starts to tackle larger, more complex sketches, he or she finds that the sketcher might add un-intended relations. This usually happens when a sketched end-point lies in close proximity to several other lines. This makes it hard to control the cursor finely enough that you can distinguish the difference between a Point-snap, a Horizontal, a Perpendicular, or perhaps a nearby Midpoint relation. Here are some general hints about how to avoid getting the ‘wrong’ relations.
1. Zoom In. If you are squinting, then you are not using Pan and Zoom effectively. “It is hard to assemble a watch, from across the room”. SolidWorks snaps to and selects points/vertices first, then lines/edges, then faces. The further out your zoom is, the more likely you will only be able to snap/select points and vertices.
2. Exaggerate. If a sketch line is to be 3 degrees off the vertical, sketch it at 30 degrees; you can easily correct the parametric dimension later. If a segment is to be .062″ long, make it 1/2″ long, and dimension to the correct size later. While it is over-sized, however, it will be far easier to draw the rest of the profile without getting false Endpoint or Midpoint snaps.
3. Trim instead of Drag. For example, if you want to vertical line attached to an edge, but you keep getting nearby Endpoint, Midpoint, or Perpendicular relations instead, draw the line grossly over-sized, so that the 2nd end is nowhere near the rest of the model. This will avoid getting any relations except the desired Vertical. Then use the Trim tool to remove the excess. (Trimming a line to another automatically creates a Coincident relation).
4. Hold down the Ctrl key while sketching. If you hold down the Ctrl key while you’re in the middle of drawing a line or arc or other sketch entity, this will temporarily disable all relation inferencing and snapping. You can then add the relationships manually.
How to Precisely Position an Un-Constrained Sketch
Sometimes a user does not wish to apply constaints and dimensions needed to fully shape and size a sketch. This could be because the data is imported from another CAD system, or it may be free-form, stylistic data (splines and such). However, it can be hard to align and locate the sketch precisely on the model, because each new constraint tugs the sketch out of shape instead of moving it. There are three good ways to accomplish this, depending on user taste, and also upon how much parametrization of the sketch you plan to eventually apply.

First, the easiest (read: lazy) way is to group-select all the lines, and choose TOOLS – BLOCKS – MAKE BLOCK. The lines are now all ‘frozen’ relative to each other, and can now only translate or rotate as a group. You may now apply sketch relations to the entire block to position it, and when finished, you may then EXPLODE the block to restore individual control to each line.

The second approach also requires that you first pre-select all the lines in the sketch. Then use the icon found under TOOLS – SKETCH TOOLS – MOVE, (you will also see the related tools ROTATE, SCALE, and COPY). These commands will allow you to position the selected lines very precisely, relative to a FROM and TO selection points, or by inputting jog distances or angles, and they result in no new parametric relations.

A third slick solution is to use Derived Sketch. A derived sketch is an associative copy of an existing sketch. It can only be positioned — it’s size and shape is always exactly the same as the original. This behavior is ideal for problems where you want to reference the original sketch several times, or where you prefer to leave the original data as a master sketch in its original location. One disadvantage of this approach is that it is all-or-nothing, you can only DERIVE a sketch that includes every line in the entire sketch, and the other two methods listed above will also work on a few selected lines.

To DERIVE a sketch, first you must exit the sketch you were working on. Now use Ctrl-select or Shift-select to choose the sketch you just exited, and also select the plane that the new sketch should be built on. With these two items pre-selected, you will be able to Insert – Derived Sketch. You will now be editing a second sketch, an associative copy of the first. You may align and position this sketch, without causing any deformation. You can now Hide the original sketch. To make any shape changes later, edit the original sketch, an the derived one will update with those changes.

Optional: You may wish to sever the link between the two sketches, and delete the first sketch. To do this, right-click the derived sketch in the FeatureManager, and select Underive. Then you can delete the earlier sketch.

Dragging Features and Sketches in 2008 with “Instant 3D”

What was old is new again! A function added to SolidWorks 99 gave the ability to edit a sketch without having to invoke the Edit Sketch command. This function is called Move/Size Features. It allowed you to reach into a sketch from the 3D model environment and drag any unconstrained sketch geometry dynamically. The function was NOT available on your Features toolbar by default, so you had to add a special icon to your toolbar. Right up until Solidworks 2007, you would have to use Tools – Customize – Commands – Features, then drag and drop the icon for Move/Size Features onto your Feature Toolbar.
The icon looked like two green dots with arrows sticking out, as shown here: This function was fun, powerful, and a little bit dangerous in terms of what it could do to some of your relations internal the sketch, (such as if you rotated the sketch plane away from the default Horizontal and Vertical directions), and so it went largely unnoticed by all but the most expert of Solidworks users.
In Solidworks 2008, this function comes out from the shadows! The programmers re-wrote the command thoroughly to make it even more powerful, and remove the hazards that it originally presented to the novice user, and the command is now called Instant3D.  The icon for this command is now found on the default Solidworks toolbars and Command Manager, and in the templates of a new installation, it will be turned ON by default. This icon is what allows you to drag on the face of any solid, and pull it in any direction not yet constrained within the sketch. If a feature does have parametric dimensions, Instant3D model will display those dimensions with a blue drag-ball at the free end of the dimension, allowing you to re-size the dimension with the aid of a ruler scale. Features not yet located parametrically can also be re-positioned within their sketch planes via dragging. If long-time users of Solidworks are a little un-nerved by the ease with which features can be re-positioned and re-sized, and wish to return to the version 2007 (and prior) edit mode where a double-click is required to edit a parameter, they need only to turn this icon OFF.

Relations for Points in a Sketch: Coincident vs. Merge
The Add Relations dialog permits two different relations for points in a sketch: Merge or Coincident. Fortunately, users need never worry about choosing one or the other — only one of these relations is ever available at a time, and the system automatically hides the other, based upon the pre-selected geometry. What is the difference between these?
Coincident applies to any point belonging to the current sketch, and a point that is referenced outside the current sketch (a model vertex, endpoint of a different sketch, etc.). Even though the two points will now co-exist in space, they retain their individual identities.
Merge applies between two endpoints or centerpoints that both belong to the current sketch. In this case, the system ‘dissolves’ one of the endpoints, and the other endpoint becomes common to both adjacent lines or arcs. This simplification greatly streamlines the management of other relations that the user may wish to apply at this point.

Why can’t I create a Sketch Point in SolidWorks at the Same Location as an Existing Point? 

When a line’s endpoint is drawn sufficiently close to another line in the same sketch – it performs a Merge (see above). When the endpoint is drawn within snapping distance of a model vertex, it captures a Coincident relation. The only exception is in the placement of a Sketch Point [Tools - Sketch Entities - Point], which you cannot place on the endpoint of a line or arc. This is prevented because the Merge relation would cause the Sketch Point to dissolve into nothing. However, for the Hole Wizard and Sketch-Driven Pattern and other situations with laying out construction sketches, the user sometimes wishes to put a Sketch Point on top of an existing endpoint.
There are actually two easy ways to place sketch points on the end of some other sketch entity:
1) Although you cannot snap a Point onto the end of a Line, you can perform the reverse. Sketch the Point first, then snap the Line over it.
2) Alternately, you can place the Sketch Point graphically near the desired endpoint, and then create a Coincident relation.
How can I Locate the Focus of a Sketched Ellipse?
The SolidWorks sketch environment lets us easily create an ellipse with a simple tool. This ellipse has a number of reference points on it to help us to locate and dimension it. Figure 1 shows what we get from SolidWorks: four vertices, and a center point. In some optical designs and other applications, the focal points of the ellipse are needed. We can add some geometry and relations to automatically locate the foci of the ellipse.

The procedure requires two construction lines sketched as follows:

5) Optionally, add a second point G and a construction line DF. Add a symmetric relationship between points E and G about line DF.

Why can’t we all just get along? Trading files back and forth is an issue that plagues engineers often. However there are some things that can alleviate the problem. Take exchanging Pro/ENGINEER parts and assemblies with SolidWorks. This works relatively well with the robust feature sets that SolidWorks offers for either handling the Pro/ENGINEER features natively as well as handling edits with explicit face manipulation.
First, let’s look at the issue of viewing Pro/ENGINEER files. SolidWorks eDrawings software, a free download, allows users to view native SolidWorks, DWG/DXF and Pro/ENGINEER parts and assemblies. If you have the eDrawings Professional package, you can also measure and markup these files, and send them to your colleagues, customers or vendors to review and markup as well. Finally, you can also download eDrawings Publisher plugins for a variety of other CAD programs, like Pro/ENGINEER so save parts, assemblies and drawings to the eDrawing file format. This publisher also works with PTC’s OneSpace Explicit modeling package (The old ME30) as well as many other CAD programs.

Once we have viewed the file in eDrawings, we can then open the file in SolidWorks for editing. SolidWorks can open the most current versions of Pro/ENGINEER Wildfire and for the latest specifics, I would encourage you to take a look the online SolidWorks help for Assembly import and Part Import. In the video embedded below, I run through several options of importing and exporting Pro/ENGINEER files with SolidWorks.

In the first part of the video, we open the Pro/E assembly in eDrawings Professional, and mark it up to indicate a design change is needed. In this case we need to change the length of the link on a toggle clamp. Once this is identified, we open the Pro/E assembly in SolidWorks. We are presented with a dialog box asking us how we want to import the assembly.



For an assembly we either have the choice of bringing in the part’s feature history or to use the BREP (boundary representation) of the parts. I choose the BREP as it is the most reliable and will bring in the most accurate representation of the solid model into SolidWorks. Plus, I get the opportunity to import mates (constraints in Pro/E). If you use the feature import, this is not a capability, however, you can import a part later with features and then replace that new part in an assembly that you have already imported.
In the following image, you will notice that the assembly comes in with all mates and material properties. Without even doing anything, it looks great. I am using SolidWorks 2011 and turned on the integrated PhotoView 360 preview and it looks fantastic, see below:


Here you can examine the mates and dynamically move the clamp as you would expect to to move. You can even turn on dynamic collision detection to see what the true range of motion is. Now we need to make the design change lengthen the link. Simply click on one of the links and choose “Edit Part” which allows you to change the part inside of the assembly model. Since I imported the part with no features, I will use the “Direct Editing” tools to lengthen the link. After making the direct edits to the link, and then testing the dynamic motion again I notice my range of motion is now limited and I need to change the clamp-base component, so I employ the direct edition tools again.
I should also note, that you can save out a versioned Pro/E assembly after you make your changes in SolidWorks, to share with other Pro/E users. Check out the video below for a full run-through and please add comments on your experience with this!

Getting Started with Simulation Tutorials in SolidWorks Premium

By default, SolidWorks Simulation does not open when SolidWorks does. We can change this by going to Tools > Add-Ins, shown in Figure 5.

Defining the material For SolidWorks Simulation Tutorials

SolidWorks is, first and foremost, a 3-D modeling tool. Look in the tutorials folder for a SolidWorks model named “glass.SLDPRT”. When you open it, it should show a wine glass, as in Figure 1. This is the model we are going to study in this tutorial. Save a copy to your Charlie account.

If you wish to practice your modeling, part of a technical drawing of this wine glass is included in Appendix A. Units are in millimeters. This should be enough information to draw your own.