NEWSUG Meeting Minutes

May 24, 2005, 5:00 p.m.

Fox Valley Technical College, Appleton, Wisconsin

While this report generally covers the meeting events, they have been arranged into a logical sequence and refined with the purpose of making them helpful without necessarily precisely representing the facts as they happened.

20 people attended this meeting.

Click on these links for easy navigation.

SolidWorks Tips

Modeling With Consideration for Drafting

Drafting Techniques

Next Meeting

Announcements – Bob Braun

The members voted on and accepted Dan Sheber as the third NEWSUG Board Member.

The results of the survey taken at the March meeting were presented. This is the survey in which the members indicated their interests in presentation topics. A complete listing of the survey results are in the March 2005 meeting minutes.

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SolidWorks Tips – Moshe Saraf

Creating Smooth Surfaces

If you design a part with tangent surfaces, the tangent points will show and the curved and tangent surfaces will have a line between them. When the multiple surfaces and tangent line are a problem for you, this tap will solve your problem.

1. Create the profile sketch like you normally do. You may need to add points or other reference geometry in order to control the resulting profile.
   
2. Select all of the segments in the profile.
   
   
3. Select the Fit Spline icon from the Spline tool bar.
   
   
4. In the Spline Tool dialog box, be sure to select the Delete geometry check box.
   
   
5. Select the OK check box and extrude your spline profile. The resulting part will be smooth with no tangent line.

Matching Colors

When you need to match a part or feature color to the color of something that exists, this process will work for you.

1. Get the object that you need to match into a digital format. This may require a digital photo it the part may already exist in a digital format.
   
   
2. Go to any of the many image editing programs. Select the color you want to match and have the program display the color numbers. In the sample problem, the colors to match a medium blue were 3, 97, 210. Record these numbers.
   
   
3. Select the part or surface that you need to have match the original.
   
   
4. Select the Edit Color icon.
   
   
   
5. In the Color and Optics dialog box, under the Color Properties section, click the Numeric check box.
   
   
6. Edit the red, green and blue numbers in the dialog box to match the values recorded in step 2.

Break Concentricity Relationships

When you sketch two circles that are inadvertently given a concentricity relationship, that relationship can be efficiently broken with these steps:

1. Press the control button and select one of the circles.
   
   
2. Drag the circle to a new location.
   
   
3. If you release the control key first, you will break the concentricity constraint relationship.
   
   
4. If you release the mouse button before the control button, you will copy the circle to the new location.

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Modeling With Consideration For Detailing – Moshe Saraf

Motivation

The reasons to bother with modeling with consideration for detailing include:

• Preserve options for design changes.
  
  
• Designer controls the full design, including dimensioning.

Model Orientation and Drawing Views

Drawing views are based on model view names, not plane names. As a result, you have the option to change view names in the model and overwrite existing view names in order to give the part a new drawing orientation. Here is a general procedure to change a view name:

1. Orient the model to show the view that you want to assign the name to.
   
   
2. Press the space bar to get the view name dialog box.
   
   
3. Select the New View icon.
   
   
4. In the dialog box, enter the view name that you want to use.
   
   
5. The new view name will carry forward to the drawing that uses that view name.

Note that if you choose the Front, Back, Left, Right, Top or Bottom views and rename them, other views that are associated with that view name will adjust.

Mark Dimensions For Drawing

By default, all model dimensions can be displayed in a drawing. To mark a dimension as one that should not display in the detail drawing, follow these steps when the dimension is displayed in a sketch or other model view mode.

1. Insure that the selection tool is selected and not the dimension tool.
   
   
2. Right click on the dimension.
   
   
3. From the drop down menu, deselect Mark For Drawing.

In many cases you will want to use this technique in combination with other techniques to give you a complete set of dimensions to import into the drawing. For example, you may need to add text to the Dimension Text to clarify that the dimension applies to more than one dimension. You can also add driven dimensions. Driven dimensions can be marked Mark for drawing like a driving dimension.

Inserting Model Dimensions

You can open a new drawing and insert a part by selecting the Make Drawing From Part/Assembly icon.

Once you have the model on a drawing sheet, insert the dimensions by going to the Insert menu and select Drawing Items. From the drop down, select Select all from the dialog box. The dialog box at the top must have Entire model selected. Select the check box.

Once the dimensions are inserted, they can be moved around to make them more useful. If you control + select a dimension, you can drag it to another view to copy it. If you shift + select a dimension, you can drag it to another view to move it.

Driven Verses Driving Dimensions

In your drawing (and in your model sketches), you can distinguish driving versus driven dimensions because driving dimensions are black while driven dimensions are grey.

Weldment Cut List

Making weldments and weldment drawings with cut lists have advanced significantly from SW 2004 to SW 2005. In SolidWorks 2005, follow these steps to create your weldment cut list.

1. Make your weldment model.
   
   
2. Insert the model in a detail drawing.
   
   
3. Go to the Insert menu and select Tables. From the drop down, select Weldment Cut List.
   
   
4. Follow the prompts for view, templates and anchor.
   
   
5. Select the check mark.

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Detail Drawing Techniques – Dan Sheber

Bringing Model Geometry into a Drawing Format

Different ways were demonstrated to bring geometry into a drawing:

• If you have both the model and a blank drawing sheet open, you can drag the model to the drawing. Once the first view is placed, other views can be dragged from the first view, including an isometric view.
  
  
  
• From the model, select the Make Drawing From Part/Assembly icon. Follow the prompts to make the remainder of the drawing.

Creating and moving views

If you have not created enough views when first putting the model in the drawing format, you can select the Projected View icon and a view to create additional views by selecting their location relative to the view you already selected.

Once a view is created, it can be dragged to a new location by moving the cursor over the edge of the view outline until it looks like a hand. Select and drag the view to its new location. Dragging cannot violate the basic view relationships unless they are explicitly broken. As long as a drawing is linked properly to a model, new views can always be projected and dragged.

You can have different model configurations in the views. To change configurations in the views:

1. “Right click” on the view you want to change.
   
   
2. Select properties from the drop down menu..
   
   
3. Toggle to the model configurations to be shown in that view.

Dimensions can be inserted through the model by selecting Insert menu, as describe above, or they can be inserted manually. Both techniques have advantages. The best method depends on how model sketches are made.

When you have more than one similar part model that need detail drawings, you can save work on the second drawing with this technique.

1. Create the first drawing from the first model. Save it.
   
   
2. With the drawing open, selecting Save As. Select Save as a copy in the dialog box. Key in the new file name. Save the new file.
   
   
3. Close all drawings and models.
   
   
4. Select Open files through SolidWorks and click the new drawing once (without opening it) in the Open dialog box.
   
   
5. Select References in the Open dialog box. This dialog box should also show a small preview of the drawing file.
   
   
6. In the next dialog box, find the model file of the new part. Double click it. This will bring you back to the “link reference” dialog box. Click the box next to the new link you created. Click Ok.
   
   
7. Click Open. Your drawing will now be linked to the new part model, and the geometry will automatically adjust.
   
   
8. Save the drawing to preserve the work you have done.
   
   
9. Tweak the new drawing to complete it.

Bill of Materials:

Before inserting a Bill of Materials (BOM) on an assembly drawing, an anchor must be created. Do this in the “Format Edit” mode with this sequence:

1. Right click Sheet Format in the drawing tree. If all the views disappear, you are in Format Edit mode where you want to be.
   
   
2. Right click an upper corner of the format, and select Anchor in the drop down menu to create the anchor point.
   
   
3. The menu will show a list of types of tables that can be anchored. Bill of Materials should be on that list. Select it.
   
   
4. Leave Format Edit mode by right clicking Sheet format in the drawing feature tree, and selecting Edit sheet in the menu.
   
   

To insert the BOM, follow these steps:

1. Select the Insert menu.
   
   
2. Select Tables from the drop down menu.
   
   
3. Select Bill of Materials from the fly out options.
   
   
4. Click on any view to activate the BOM window of properties and adjustments.
   
   
5. Select how to anchor your BOM to your anchor point. You can also adjust rolls and columns in this window along with other adjustments as desired.
   
   
6. Select the check mark to finish.

Hole tables

Hole tables are a table that creates an identification for each hole in a view, the hole size and the vertical and horizontal coordinates of those holes. For example, a mounting plate or side frame have many holes on a large flat area and are ideal for this feature. Create a hole table with these steps:

1. Create an anchor in your sheet format like you did with the Bill of Materials if you want a specific hole table location. Alternately, you can place your hole table in any open drawing area.
   
   
2. Select your origin point for all dimensions. This is usually the lower left corner of the part.
   
   
3. Select the surface where all the holes pierce first. This is usually the sketch plane use by all of the hole wizards. This surface must be in the same view where the origin was selected earlier.
   
   
4. Under the Insert menu, select Tables and then Hole Table.
   
   
5. Follow the prompts in the dialog box to locate the anchor and make other customizations.
   
   
6. Select the check mark to close the dialog box.
   
   
7. Locate the hole table.

Next Meeting

The next NEWSUG meeting is scheduled for September 6, 2005. We plan to use sheet metal design as the featured topic.

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