SolidWorks Tech Tips – Part Modeling

When I drop a Library Feature, like a Sheet Metal Stamping Tool, into a Part, I Cannot Get it to Rotate 90 Degrees from Where it Originally Landed.

Sketches usually contain a lot of Horizontal and Vertical (H, V) relations. But when you drop a feature into a new part, the base sketch will re-orient itself to the target plane’s H and V directions, thus preventing you from being able to rotate the sketch. The real problem here is that, face by face, the choice of the H and V directions is a fairly arbitrary one, dependent upon hidden rules in the software.

Solution 1: Set your own baseline
When constructing a Library Feature, for example a Sheet Metal Stamp, do NOT use Horizontal and Vertical relations. Instead, pick one line (or construction line) in your sketch as a baseline for determining orientation. Make the first line at some exaggerated angle away from horizontal, to avoid getting H or V snaps. Have all your other lines relate to it with Perpendicular or Parallel relations. When you deploy the stamping tool into a part, you will be able to orient it to any angle, by putting a relation (H, or V, or Parallel, or an Angle dimension) to that base line.

Solution 2: Override default H and V relations
If you’ve already built a complicated sketch and it is already riddled with H and V relations, then Solution 1 above is not so fun. Imagine that each sketch is a set of lines lying on it’s own sheet of clear mylar – your usual Sketch relations and editing commands restrain how the lines relate to each other, relative to the mylar sheet’s (0,0) corner.

You can over-ride the H and V relations in the sketch using the command under TOOLS –> SKETCH TOOLS –> MODIFY. This will pull up a dialog that allows you to drag, rotate, and even scale a sketch, provided that you have NOT YET ADDED ANY RELATIONS or dimensions that would locate the sketch in space. But the MODIFY command ignores all the relations within the sketch, and instead allows you to grab the corners of the entire mylar sheet, and slide or rotate the sketch in space – and the H and V relations slide along with it. In the case of a sheet metal tool, you usually only have to rotate the sketch +/- 90 degrees in this dialog, then you close it and add dimensions to finish the location.

What happens if you HAVE already added relations to locate in space? The MODIFY command throws a warning message that the sketch is not free to move.

How Can I Make Individual Part Files from a Multibody Part?

SolidWorks 2004 introduced the ability to work with multibody parts (parts with more than one continuous volume) This can be useful to develop designs that are more easily conceptualized and modeled using a single part file, but will be manufactured as an assembly of parts. This is sometimes referred to as the “master model” technique.
To create separate part files for each of the bodies in a multibody part file, follow these steps:

1. Create the multibody part. [Look for keyword “multibody” in the SolidWorks Help index for more about this step.]

2. Choose Insert – Features – Save Bodies. Since you already have multiple bodies in your part, you do not need to select a Trim Tool for the Split feature. (Note – prior to Solidworks 2007, you didn’t have Save Bodies, and would instead select the Split command. Then as now, the Split can also be used to spawn part files from each selected body, even if no actual cutting had been done within the Split dialog).

3. Within the dialog, click on one of the callouts seen in the graphics window to designate a filename and location for the part file for that body. (Or you can double-click in the list of Resulting Bodies in the PropertyManager).

4. Repeat step 3 for all the bodies for which you wish to create new part files.

5. (Optional) Select Consume Bodies in the PropertyManager ONLY if you wish the spawned body to disappear at this point from the master model.

6. Click the green OK button. The new part files have been created. They will update associatively when the original part is changed.

7. (Optional) Right-click on the Save Bodies feature in the FeatureManager and choose Create Assembly. Click “Browse” to specify a name and location for the assembly. Click OK to generate a new assembly using the part files created in step 6. Each part comes into the new assembly in a Fixed state, aligned to the assembly origin. Since the parts were all derived from the same origin in the first place, they all end up in the exact correct locations in the new assembly.

8. Save all open documents.

Loft to a Point

Many of our customers have learned about SolidWorks’s Loft feature in training. A Loft combines two or more cross sections (profiles) to produce a free-form solid. Here is a lofting option you may not be aware of. It is possible for one of the profiles of the loft to be a single sketched point. This is useful in creating shapes that taper down to zero.

Try this example:

1. Open a new part.

2. Sketch a 2″ diameter circle on the Front plane, centered on the origin. Exit the sketch.

3. Create an offset plane 2″ from the Front plane [Insert – Reference Geometry – Plane].

4. Open a second sketch on the offset plane. Sketch a point coincident to the origin [Tools – Sketch Entity – Point]. Exit the second sketch.

6. Loft from the first sketch to the second [Insert – Boss – Loft]. You will get a cone shape.

7. Now try this option: Edit the Loft [right-click – Edit Feature]. In the region of the PropertyManager labelled “Start/End Constraints”, choose “Normal to profile” for the point, and your cone will get a rounded end.

Activating the “Link to Thickness” Option.

Many SolidWorks Users use the link to thickness option for extrusions and cuts in a sheet metal part but may not realize that you can activate this option without having any sheet metal features in your model. Link to thickness is an option that can be widely used in many other model types, not just sheet metal. Activating the option is as easy as 1, 2, 3.

1. Right-click on a model dimension you would like to designate as the thickness.

2. Select Link Values from the pop-up menu.

3. Enter the name “Thickness”.

The Link To Thickness option is now available in any extrusions you create or edit.

How Can I Measure the Overall Height of an Irregular Surface?

Imagine that you have a model that has spline-based surfaces, rather than planar or analytic faces, at the height, length, or width extremities. Or perhaps the highest point on your model is a face resulting from a fillet, rather than an extrude, revolve, etc. How can you measure the overall height?

The Measure tool will allow you to measure to an irregular surface, but it will only tell you the minimum distance to the surface, not the maximum. So, create an offset reference plane that lies well beyond the maximum height of the irregular surface. Make the distance between the bottom of your part and this new plane an easy, round number (let’s call this X). Then, use Tools – Measure to measure the minimum distance from the irregular surface to this new reference plane (let’s call that distance Y). The overall height of the model = X-Y.

Use this trick twice if the part is irregular at both ends.

How to Extrude “Up To” or “Offset From” Multiple Faces

Both Insert – Boss – Extrude and Insert – Cut – Extrude features allow you to use a target face as either an Up To or an Offset From end condition. But you can only select one item at a time for the target in the Extrude dialog. What if the extruded feature is going to overlie more than one face?

The solution is to use Insert – Surface – Knit. Prior to creating the extrude, use Knit to gather together all of the faces that the extrude is going to contact. This will result in a single surface object in the FeatureManager. Then, when you are in the Extrude dialog, select the resulting knit surface by clicking on it in the FeatureManager.

Creating a Pattern with “Skipped” Instances

Often, components will have features that can be arrayed, but the array is not perfectly consistent — there are some copies in the pattern that you don’t want. There are two easy ways to do this in SolidWorks.

Method 1 (SolidWorks 2001 and later): Create the pattern as you normally would, but before you click OK, scroll down the PropertyManager dialog to find the option for Instances to Skip. Click in this option box. You will now see colored dots in the graphics window over each instance (copy) in the pattern preview. Click a dot to change its color and remove that instance from the copy.

Method 2: After the pattern has been created, you can select one or more instances and hit the Delete key. A dialog will appear that gives you two choices – eliminate the entire pattern (not what we want), or eliminate only the selected instances from the pattern.

In either case the next time you Edit Feature on the pattern, you will see that the skipped instances are now listed in the Instances to Skip option box. You can delete items in that list to add them back into the pattern, or you can click the colored dots to turn the instance on again.

Dragging and Dropping Features in the FeatureManager

In Solidworks 99 and prior, while dragging a feature in the FeatureManager to re-order it, you had to make sure that neither the feature you were dragging, nor the feature you were dropping it after, was expanded to show their ingredient sketches, etc. If you forgot to collapse the FeatureManager, the error message “drag and drop failed” appeared.

In SolidWorks 2000, this was corrected. However, users are still sometimes disconcerted by seeing the “do not drop” cursor (the circle with the diagonal slash through it) when trying to reorder a feature after another, if the latter is expanded to show its sketch. Do not lose faith – you can still reorder these features! All you have to do is position the cursor just after the feature icon, but just before its sketch icon. It may seem as though you are trying to drop between the feature and its sketch, but in fact that can’t happen. Because the system knows you cannot re-order a sketch that is inside another feature, it treats that area of the FeatureManager as dead space, and that is why you cannot drop anything there. But just nudge your cursor above the expanded sketch, and the reorder will work correctly.

Can I Create a Configuration of My Model Using the Rollback Bar to Remove Some Features From My Model?

SolidWorks configurations do not currently recognize the rollback bar as a means for removing features from a configuration. The features need to be removed by suppressing them. One way to suppress a feature or features is to select the feature or features to be suppressed then choose Edit – Suppress – This Configuration. Note that you can use a Shift-select in the FeatureManager to select all the features at the end of the tree for suppression, to mimic the effect of the Rollback bar.

How Can I Make Individual Part Files from a Multibody Part?

SolidWorks 2003 introduced the ability to work with multibody parts (parts with more than one continuous volume) This can be useful to develop designs that are more easily conceptualized and modeled using a single part file, but will be manufactured as an assembly of parts. This is sometimes referred to as the “master model” technique.

To create separate part files for each of the bodies in a multibody part file, follow these steps:

1. Create the multibody part. [Look for keyword “multibody” in the SolidWorks Help index for more about this step.]

2. Choose Insert – Features – Split. Since you already have multiple bodies in your part, you do not need to select a Trim Tool for the Split feature.

3. Within the Split command, click on one of the callouts seen in the graphics window to designate a filename and location for the part file for that body. (Or you can double-click in the list of Resulting Bodies in the PropertyManager).

4. Repeat step 3 for all the bodies for which you wish to create new part files.

5. (Optional) Select Show Bodies in the PropertyManager. This will keep the solids visible in the current part file.

6. Click the green OK button. The new part files have been created. They will update associatively when the original part is changed. 7. (Optional) Right-click on the Split feature in the FeatureManager and choose Create Assembly. Click “Browse” to specify a name and location for the assembly. Click OK to generate a new assembly using the part files created in step 6. Each part comes into the new assembly in a Fixed state, aligned to the assembly origin. Since the parts were all derived from the same origin in the first place, they all end up in the exact correct locations in the new assembly.

8. Save all open documents.

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