user 2006-6-29 09:41
24 Soldiworks Tech Tips - Modeling
Don';t double-click to select a sketch plane Don';t double-click to activate a sketch plane. If you double-click on a plane it will be deselected, although the plane will stay highlighted. If you have not activated a sketch plane, SolidWorks will default to the "front" plane (plane1) if you start sketching in a blank part or assembly. Joe
Sketching - avoiding accidental references
The Solidworks Sketcher saves time and assists the new user by automatically capturing about half of the relations in a sketch automatically. However, as a user gains experience, and starts to tackle larger, more complex sketches, he/she finds that the Sketcher can frequently find and enforce 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. Below are some general hints about how to avoid getting the ';wrong'; relations.
1) ZOOM UP. If you are squinting, then you are not using PAN and ZOOM effectively. "It is hard to assemble a precision watch, from the other side of the room".
2) EXAGGERATE. If a sketch line is to be 3 degrees off the vertical, sketch it at 30 degrees; you can correct the size later, while dimensioning. 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 connect other lines to it, without getting false Endpoint or Midpoint snaps.
3) TRIM instead of DRAG. If you want to connect a VERTICAL line onto another, but you keep getting nearby Endpoint, Midpoint, or Perpendicular relations instead; Draw the vertical 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 enforces the Coincident relation).
4.) Create lines well oversized, getting only the H or V or Perpendicular, etc. Then trim back to get the line or point coincidence. Keith
Modeling advanced shapes.
Many of our customers have learned about SolidWorks’ 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:
Another choice you have in creating lofts is to loft to a sketched point. This is useful in creating shapes that taper into a point.
Try this example:
1. Open a new part.
2. Sketch a 2" diameter circle on the Front plane, centered on the origin. Close 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]. Close the second sketch.
6. Loft from the first sketch to the second [Insert/Base/Loft]. You will get a cone shape.
Try this option in the above example: On the Advanced tab of the Loft dialog box, choose "Normal to profile" for the point and your cone will have a rounded end that looks like a nose cone. Keith
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.
A slick solution is provided by the DERIVED SKETCH. A derived sketch is an associative copy of the base sketch, and as such, can only be positioned - it’s size and shap is rigid. This behavior is ideal for solving the problem stated above.
First, close the sketch you were working on. Group-select (using the Control key) both the sketch, and also the face (or plane) it lies on. Now execute the command "INSERT - DERIVED SKETCH". You will now have a second sketch, an associative copy of the first. Edit this sketch, and you will find that you may align and position, without causing any deformation. You can now hide away the original sketch. To make any later shape changes, edit the first sketch, not the derived one.
Optional: You may wish to sever the link between the two sketches, and delete the first sketch. To do this, right-click over the NEW sketch in the Feature Manager, and select "UN-DERIVE SKETCH". Then you can delete the earlier sketch. Jason
Where did the Insert - Sketch From Drawing function go in SolidWorks 2000?
In Solidworks 2000, there is no longer a pull-down menu to insert lines from a drawing into an open sketch. Why? In the latter releases of Solidworks99, they extended the "Ctrl-Drag" ability to allow a group of lines selected within a drawing, to be dragged directly into an open sketch, without the need of the Insert command. For the 2000 version, they decided the menu was redundant.
However, there is a fly in the ointment. What if the drawing view you wish to copy contains not only sketch lines, but also dimensions, notes, etc? The old Insert function allowed you to window-select your lines, and it would filter out and ignore any text or dims. The new Ctrl-Drag method does not allow text and dims to be included. So, to get the new method to work like the old, you have to turn on your filter toolbar, and filter on "Sketch Segments". Then the Ctrl-Drag will work normally.
Sketch Editing with 3D Preview
Most users know that the Move/Size Feature icon to drag a feature';s base sketch, without leaving 3D mode. This allows the user to see the 3D effect of the drag. But did you also know that, as long as this icon remains depressed, you can also enter 2D sketch-edit mode? To achieve this, first press in the Move/Resize Feature icon, (in the Features toolbar). Then, expand the feature manager to see the icon for the sketch you wish to edit, and double-click on that sketch. This gives you the complete suite of sketch creation and editing tools, and the 3D preview of the resulting feature still remains visible.
Relations for points in a sketch: Coincident vs. Merge
The Geometric 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 grays-out the other, based upon the pre-selected geometry. COINCIDENT: This relation applies to any point belonging to the current sketch, and a point that is referenced from 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 identity. MERGE: This relation applies between two endpoints that both belong within 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.
Point snapping and the SolidWorks Sketcher
Veterans of previous CAD systems sometimes assume that the Sketch Grid must be displayed, in order to assure
that adjacent line elements remain perfectly connected. This is not necessary - the Solidworks sketcher is always
in "Point Snap" mode, with or without the Grid. When a line';s endpoint is drawn sufficiently close to another line in
the same sketch - it performs a Merge. 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, 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, anyway. However, when the user is laying out a construction sketch for an irregular pattern, the user sometimes wishes to accomplish this. How?
There are actually two easy ways to place sketch points on the end of some other sketch entity. 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.
Alternately, you can place the Sketch Point graphically near the desired end-point, and then create a Coincident relation.
Either way, the Sketch Point retains its identity, (rather than dissolving, as a Merge relation would do).
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 the sheet metal feature in you 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 mouse click on a model dimension you would like to designate as thickness.
2. Select Link Values from the menu.
3. Enter the name “thickness”.
Your “Link To Thickness” option is now active.
What is the best way to create a right-hand and left-hand version of the same part design?
One approach is to create a new configuration and then “Mirror All “. But another option not always considered is the use of derived parts.
The derived part approach uses three part files to maintain the designs:
· A common part, which has geometry common to both the right-hand and left-hand parts.
· A right-hand part, which is an associative copy of the common part, plus additional features unique to the right-hand side.
· A left-hand part, which is an associative mirrored copy of the common part, plus additional features unique to the left-hand side.
Here';s the technique:
1. Model the common part. This part has features that you would like to see in both the right- and left-hand versions of your design. Save. [We';ll call this "common.sldprt".]
2. Open a new part. Choose Insert, Base Part... Browse to find "common.sldprt". Save. [We';ll call this "right-hand.sldprt".]
3. Open "common.sldprt". Pre-select a flat face of the model to reflect about. Choose Insert, Mirror Part... Save. [We';ll call this "left-hand.sldprt".]
Working with the three files:
"Common.sldprt" is termed a "base part". Any changes made to "common.sldprt" will propagate to both "right-hand.sldprt" and "left-hand.sldprt". "Right-hand.sldprt" and "left-hand.sldprt" are termed "derived parts". Changes to the two derived parts do not affect the base part, or each other.
Therefore, any design changes or feature additions that you want to make to both hands of the part should be made to "common.sldprt". Anything that you want to change about the right-hand, but not the left-hand, should be made to "right-hand.sldprt", and vice versa.
While Configurations and the Mirror All feature can be used to great mirrored parts, the chance for user error in managing which changes and features apply to which configurations (RH, LH, common) is much greater. We thus recommend this alternative as a Best Practice.
Further information about working with derived parts can be found on page 5-16 of the SolidWorks 99 User';s Guide.
How can I measure the overall height of an irregular surface?
Imagine that you have a model that has Spline 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 to measure the overall height?
The MEASURE tool will allow you to select a plane, (or planar face), and an irregular surface - but it will only tell you the minimum distance, not the maximum. So, create a (temporary) reference plane that lies well outside the part. Make the distance between your base-plane and this new one some easy, round number, (call this D1). Then, use TOOLS - MEASURE to measure the minimum distance from the model to this outside plane, (call this D2). The overall height of the model is then D1 - D2. Use this trick twice if the part is irregular at both ends.
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. Note in Figure 2 that two vertices lie on the major axis AC of the ellipse (the longer diameter) and two lie on the minor axis BD (the shorter diameter). How can we add some geometry and relations to automatically locate the foci (E, G) of the ellipse?
http://www.capinc.com/pages/support/images/pic1.gif
http://www.capinc.com/pages/support/images/pic2.gif
1) Sketch the construction line AF from one of the vertices of the major axis to the center of the ellipse. This line represents half of the longer diameter.
2) Sketch the second line DE with one endpoint on the vertex of the minor axis and the other endpoint coincident to the line AF drawn in step 1 above.
3) Set these two construction lines equal by adding a geometric relation
http://www.capinc.com/pages/support/images/pic3.gif
4) The free endpoint E of the second line is a focus of the ellipse!
5) Optionally, add a second point G and a construction line DF. Add a symmetric relationship between points E and G about line DF.
http://www.capinc.com/pages/support/images/pic4.gif
http://www.capinc.com/pages/support/images/pic5_000.gif
Why is this true? Well, recall some high school analytic geometry: an ellipse is a collection of points for which the sum of the distances from two specific points (the foci) is a constant. In other words, if I travel from focus E, to any point on the ellipse, and then to focus G, the distance traveled is the same no matter what point on the ellipse I travel to.
So, imagine now that we travel from point E, to vertex A, and then across to point G. This distance (EAG) is equal to 2AE + EG. Since EG = 2EF, this distance is equal to 2AE + 2EF, or 2AF. Now imagine that we travel from point E, to vertex D, and then to point G. Because of symmetry, DE = DG, so this distance is equal to 2DE. Due to the properties of an ellipse, if E and G are foci, the two distances must be constant. This means 2AF = 2DE, or AF = DE. The reverse is also true: by setting AF equal to DE, points E and G are the foci.
How to extrude UP TO, or OFFSET FROM, multiple faces
Both INSERT, BOSS, EXTRUDE and INSERT, CUT, EXTRUDE commands allow you to use a target Face as either an UP TO or an OFFSET FROM target. But you can only select 1 item in the Extrude dialog for the target. 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 Feature Manager. Then, when you are in the Extrude dialog, select the KNIT result by clicking on its feature representation in the Manager. (Don';t click on the graphical representation of the Knit - you will still only get a single face that way).
Detecting Invalid Sketches
Once a sketch is created for an extrude or revolve, users often use TOOL - SKETCH TOOLS - CHECK SKETCH FOR FEATURE, to determine if there are any flaws that would prevent use. However, one type of flaw is detected by the graphics processor on-the-fly.
Creation of a three-way junction of lines may eventually yield the error message, "... an endpoint is wrongly shared by multiple entities". If you have a flaw of this type, you will notice that at least one of your sketch lines changes thickness, going as thin as if it were a dimension witness line. The thin line is adjacent to the problem endpoint, and if you trim away the offending line(s), it will change back to normal thickness.
How to re-position IGES or DXF sketch data, (alternate method - see Tech Tip #16)
In a complex sketch, the technique shown in #16 can behave unpredictably. When you ';drag'; the sketch, only a few lines react, by deforming instead of translating. Using the CTRL key before hitting the left-mouse button to do the drag will normally solve the problem. There is another way to accomplish the desired end result that takes a few more steps to perform but does not rely so much on mouse technique.
After you have used INSERT - SKETCH FROM DRAWING, close the sketch. Now use CTRL-select to pre-select the sketch you just closed, and also the Plane that the sketch was built on. With both of these selected, you will be able to INSERT - DERIVED SKETCH. Derived sketches have exactly the behavior we are looking for - you can only re-position them, you cannot re-size or re-shape them. Select the sketch and move it using either dragging, or geometric relations, to position this sketch anywhere you want. Once you are done, close the sketch. Right-mouse click over this sketch';s icon in the Feature Manager, and you will see a function to UN-DERIVE the sketch. This will sever the links to the original, out-of-position sketch, and you may then delete it. (Keith Pedersen) 9/3/99
How can I measure the overall length of a 3-D Sketch?
If you open the Measure Tool, and then identify the sketch, you will have to manually select on each line segment comprising the sketch. For reasonably complex sketches, a much faster method is as follows:
Edit the 3D sketch. While in Edit mode, activate your Selection Filter, and set it to only select Sketch Segments. (This is done to avoid getting any Endpoints, which have zero length). Now group-select the entire sketch by dragging a "bounding box" around all elements. Now that the desired elements are pre-selected, open your Measure Tool, and the overall length is already computed. (Per Hoel, Keith Pedersen)
How to re-position sketch data imported (.dxf/.dwg) from a drawing
(Also see #20) When 2D lines are imported from a drawing, (via INSERT-SKETCH FROM DRAWING), the sketch lines are almost always shifted to the right and above the origin of the desired sketch plane. This happens because AutoCad places the (0,0) origin point of drawing data at the lower-left corner of the drawing sheet. Users often attempt to use the MODIFY - SKETCH ORIENTATION icon to correct this. However, this icon was intended to solve a different problem - it causes the sketch origin to move relative to the geometry, rather than the geometry move relative to the origin, (or relative to the part).
Instead, perform a window-select to group the entire set of sketch lines, and then use a Control-Drag to re-locate the lines. If you begin the drag with your cursor over a sketch point, the drag operation will allow that point to ';snap'; to the origin. The reason for using a Control-Drag (instead of a Shift-Drag, which would not leave a duplicate behind), is that the Shift-Drag action invokes the sketch dynamic solver, and will result in dragging only one sketch entity, (i.e., it ignores the group-selection). Because you are holding the Control key, this will actually result in a copy of the lines, but the extra copies are then easy to delete.
Creating Custom Bend Tables for Sheetmetal Parts
Many sheetmetal shops have developed custom bend tables for sheet metal unfolding. SolidWorks allows you to use these table values in lieu of the standard "K" values, so that when you unfold a solid part the offsets will be correct.
You can create or edit a bend table using a text editor. The files are saved as an Excel spreadsheet file, in the lang/english directory of your SolidWorks installation.
How can I unfold sheetmetal parts using custom offsets?
Many sheetmetal shops ask for models in the bent-up wireframe state. This is because many solids-based sheetmetal packages can only use the K-factor method of creating offsets. But SolidWorks does not share this limitation.
When inserting sheetmetal features in SolidWorks, the user has three choices to dictate how SolidWorks will calculate how the bend region will flatten out:
1.Use a user specified bend allowance (BA).
2.Use a bend table (where BA is extracted from the table based on the part thickness, bend radius, and bend angle - see below).
3.Calculate the bend allowance using a user specified K-factor.
If the user decides to use K-factor, SolidWorks determines the dimensional values for flattened sheetmetal parts using neutral plane calculations. This neutral plane is a surface plane internal to the piece that does not deform in any way during the bending process. The position of the neutral plane is determined by the user-defined K-factor.
If you work regularly with a shop, or you are a sheetmetal shop receiving SolidWorks models, you can define your own material, with the appropriate method for determining offsets with your manufacturing methods.
Creating a Pattern with "skipped" instances
Often, components will have features that can be arrayed, but the array is not perfectly consistent - there are "skipped" instances. You cannot select a particular instance for ';skipping';, if the instance does not really exist yet!
First create your pattern without any skipped instances. After hitting GO, select one or more instances of the pattern that you really wish to skip over, 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. The next time you perform an EDIT DEFINITION on the Pattern feature, you will see that the skipped instances are now listed in the ';skip sequence'; dialog box.
What are some techniques to place irregular patterns of multi-pass holes in plates or blocks?
Prior to Soliworks 2000, irregular patterns required several manual steps. The first step was to create a sketch on the desired face, locating and dimensioning Sketch Points at each hole location. Upon closing the sketch, the Hole Wizard was used to create desired hole geometry, on the face, in close proximity to one of the sketch points. Finally, the user had to CTL-Drag copies of the hole, snapping each on in place over a point in the sketch.
Solidworks 2000 introduces the "Sketch Driven Pattern", automatically activated from within the Hole Wizard, which combines all these steps into a single flow! The only trick is that the order of acquisition is reversed, as follows;
1) Pre-select a face to place the hole upon
2) Use INSERT - FEATURES - HOLE - WIZARD to choose the type and size of hole
3) After sizing the hole, hit the NEXT button. The "Hole Placement" dialog appears, prompting you to either place or dimension Sketch Points. In fact, you have been inserted into an open sketch, and the Sketch Point icon has been pre-selected for you. Each point you place within this sketch, will locate another hole. Once you have laid out the irregular pattern of points, press the FINISH button, and the pattern is complete.
Dragging and dropping features in the Feature Tree
In Solidworks ';99 and prior, while dragging a feature in the Feature Editor to re-order it, you had to make sure that neither the feature you were dragging, nor the feature you were dropping after, was ';expanded'; to show their ingredient sketches, etc. If you forgot to COLLAPSE the Feature Editor, the error message "DRAG AND DROP FAILED" appeared.
In Solidworks 2000, this has been corrected. However, users are still sometimes disconcerted by seeing the "Do Not Drop" cursor, (the circle with the diagonal slash thru it), when trying to reorder a feature behind another, if the latter is expanded to show its sketch. Do not lose faith - the reorder will work! All you have to do is position the cursor just after the feature';s icon, but just before the sketch';s icon. It may seem as though you are trying to place the new feature between the old feature and its sketch, but in fact that can';t happen. Because the system knows you cannot re-order a sketch that is "owned" inside of a feature, it treats that area of the Feature Manager 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 consideration for that 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 Edit, Suppress.