Dimension Type setting (Drawings)

Often on support customers come to us with drawings that have incorrect dimension values on drawing views.

More often than not the issue is related to a setting in drawing view property manager. The setting is located toward the bottom of the view property manager called “Dimension Type”.



SolidWorks® Help Files definition:
Dimensions in drawings are either:

• True Accurate model values.
• Projected 2D dimensions.

The dimension type is set when you insert a drawing view. You can view and change the dimension type in drawing view Property Managers.

The rules for dimension type are SOLIDWORKS specifies Projected type dimensions for standard and custom orthogonal views and True type dimensions for isometric, dimetric, and trimetric views.
If you create a projected or auxiliary view from another view, the new view uses Projected type dimensions, even if the original view used True type dimensions.

So if you’re adding dimensions to a view and are finding them to be incorrect?
This can occur if the drawing views are using “True” dimensions instead of “Projected” dimensions.  In general, conventional drawing views should use projected dimensions; true dimensions should be used for 3D views such as isometric and diametric.

Note: if you change this dimension type setting you will lose all dimensions that you’ve already placed in the view.

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Create Library Features From Scratch

Creating Library Features from scratch is a VERY valuable technique to know. It can save you tons of time when you have “common features” that you want to reuse over and over again.
In this case let’s say we have a drafted, filleted, pocket that we are tired of creating over and over every day. (Fig. 1) We would like to “capture” this feature into the Design Library so that we can just Drag & Drop it into any model.

1. MODEL THE FEATURE ONE TIME…

Yes. You do actually have to build it one time. When you do, consider if you want it to be “locked down” with some locating dimensions, or if you want it to remain “free” to position anywhere. If you do add dimensions to locate the feature (from the side and bottom edges in this case) then you are laying an extra requirement on the end user that they will have to identify those references (edges in this case) when they use it. This action is really repairing the dangling relation/dimension that comes in with the feature.

2. (optional) RENAME THE IMPORTANT DIMENSIONS TO LOGICAL NAMES…

This step is totally optional, but sure does make the part a lot more user friendly. If you just leave everything named “D1@Sketch3” and “D4@Cut-Extrude2” that isn’t going to make a lot of sense to anyone who goes to use this Library Feature.  If you right click on the Annotations folder in the Feature Tree and turn on “Show Feature Dimensions” (Fig. 2) this will display ALL of your part dimensions on the screen. Then if you also turn on “view dimension names” from the heads up view toolbar (Fig. 3), you can see the names that were auto assigned. Now you can just select a dimension and over in the Property Manager give it a new name. Or you can double click a dimension and change its name right there. (Fig. 4) You of course only need to worry about renaming the dimensions that you are actually going to use in the library feature. In this example we wouldn’t need to worry about renaming any of the dimensions in the big block. Only those in the “pocket” features.
  

3. (optional) CHANGE THE COLOR OF THE ACTUAL FEATURE(s), AND ORIENT…

In the Feature Tree, Ctrl+select the features that make up the library feature you want to create. After you let go of the Ctrl key, on the pop up toolbar will be an appearance icon (color ball). (Fig. 5) Use this to change the FEATURES to something that stands out. You could also change the rest of the part to something like gray or white. This is just going to make the thumbnail graphic show better in the Design Library. Next you would want to orient your model to however you want the thumbnail graphic in the Design Library to look. However, there is a setting you most likely want to turn OFF. It is Document Properties—Image Quality (Fig. 6)

4. ADD TO LIBRARY…

Open up the Design Library in the Task Pane and navigate to the folder you want to store your new library feature in. Hit the “Add To Library” button at the top. (Fig. 7) In the property manager that comes up on the left, under “Items To Add” (Fig. 8), BE SURE to select which features you want included in the Library Feature! (use the flyout feature tree). For example in this model we would select everything EXCEPT the first feature (the big block that we cut the pocket into). If you included that block then it would also get inserted when you used the Library Feature rather than just the pocket with the fillets. A lot of people miss this step. By the way, you could of course PRE-select the features in the feature tree BEFORE hitting the “Add To Library” button if you wanted… Hit OK to finish adding the features to the library.
     

5. ORGANIZE/CLEAN UP THE LIBRARY FEATURE…

You should now be in a “.sldlfp” (library feature part) file now. Look in the Feature Tree. There should be green “L”s on all of the features that you intended to be included in the library feature. (Fig. 9) The library feature is really ready to use, but there is some “clean up” work that should be done in the file first. Open up the “REFERENCES” and “DIMENSIONS” folders in the Feature Tree. (Fig. 10) The References folder shows what the user will have to “satisfy” when using the feature. In this example the user will drag & drop the feature onto a face to satisfy the Placement Plane, and then they will select two edges to position the feature. These two edges are required because we DID put positioning dimensions to some edges of the block in the original part. If we had left the original feature “free” to move, we would not have this requirement in the Library Feature. In the Dimensions folder, drag any dimensions that are considered “locating dimensions” into the Locating Dimensions folder (i.e. the two dimensions from the edges of the block). By default when the library feature gets used, any of the other dimensions listed in the Dimensions folder will be able to be modified as the feature is placed. This is very nice to be able to modify the feature on the fly on a case by case basis. However, if you want to lock the user out of being able to modify certain (or all) of the dimensions of the feature, drag those dimensions into the Internal Dimensions folder. In our example we have locked the user out of being able to change the Draft Angle and the Corner Radius of the pocket. (Fig. 10)

 Now Save the .sldlfp file one more time, and then close all open files.
     

6. YOU’RE DONE! TRY USING YOUR LIBRARY FEATURE !!!

Have fun creating an infinite number of Drag&Drop features in your library to save you tons of time!

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How to Modify Sketch

 

SOLIDWORKS has many tools that are often forgotten because they are not on the main toolbars, or talked about much in training classes. One of these tools is the Modify Sketch tool, which has 3 main functions for modifying your Sketch, including Moving/Flipping, Rotating and Scaling.

Modify Sketch can be found in the Tools dropdown, under Sketch Tools, Modify…

To Move a sketch you have two options the first is to enter a Translate value into the dialog box.  The other option is to move a sketch in the graphics area, using the pointer:

• Press the left-mouse button  to move the sketch.
• Point at the end points or center of the black origin to display one of three flip symbols. Right-click to flip the sketch on the X axis, the Y axis, or both.
  •  Flip sketch along X axis
  •  Flip sketch along Y axis
  •  Flip sketch along both axes

To Rotate a sketch you have two options the first is to enter a Rotate value into the dialog box. The other option is to rotate a sketch in the graphics area, using the pointer:

• Press the right-mouse button  to rotate the sketch around the black origin.

Note: The speed you use to rotate determines by how much the angle increments. Slow motion increments the angle one degree at a time; quicker motion increments the angle by ten or more degrees at a time.

• Point at the center point of the black origin to display a point symbol . Click and drag the center of rotation independently of the sketch, then rotate the sketch around the black origin.

Lastly to Scale a sketch select either the Sketch origin or the Movable origin from the Scale About in the dialog box. Once you choose what to Scale About enter a Scale Factor and press enter.

One last item to remember is that you cannot Modify a sketch that has external references, if your sketch has external references you will see the following message and will not be able to access the command until you delete those references.

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Using the Modify Configurations Table in SOLIDWORKS [VIDEO]

 

For many users, both new and more experienced, working with files with multiple Configurations can get very complicated and confusing, especially if several different variables are being controlled in the various configurations.  To help manage this, one thing I recommend to all my students starting out with configurations and to anyone who contacts us for help at our support desk, is to ALWAYS use the Modify Configurations table ANYTIME they are working with configurations.  There are other ways to work with configurations, such as design tables or manually adjusting each value, but the Modify Configurations table is often the perfect balance of speed and control for working with either simple or highly complex sets of configurations.  The benefit of using a table is that you are able to see all of your configurations laid out together with their individual settings and/or values.  This makes troubleshooting and error checking very easy.

To start a Modify Configurations table, right-click on any feature, dimension, mate or component and select the “Configure Feature”, “Configure Dimension” or “Configure Component” command.

Different Configure Commands

 

Once the table is launched new features, mates or components can be added to the table by double clicking on them in the FeatureManager Design Tree area.  New dimensions can be added by showing them in the graphic preview area and then double clicking on them to add them to the table.  New configurations can be created directly in the table and their individual settings adjusted then applied to the SOLIDWORKS model.

Modify Configurations Dialog

 

One important thing to remember though about the Modify Configurations table is that it is simply a view, a way to see all of the configuration data in one place.  If you close the dialog without saving the table view, it’s gone, and you will need to recreate that view of the data again.  To avoid this, once you have added all of the columns in the table (even if you haven’t completed creating all of the configurations yet, or haven’t made all of the adjustments for each configuration) save the table view right away.  You will need to give the table view a name then click the “Save Table View” button.  This will add the table to a special folder on the Configuration Manager tab.

Save Table View

 

Double-clicking the table in that folder will bring up the column set up in the Modify Configurations table again.

Access the Saved Table

 

Here is a video demonstration of modifying configurations with a Table:

 

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Right Sketch, Wrong Sketch Plane

How many times have you created a sketch and then figured out that it’s on the wrong sketch plane or face.  Even after all the years that I have being using SOLIDWORKS I still do that.  You have the ability to move a sketch to a different plane/face with about 3 mouse clicks.
First you need to be out of the sketch.  You don’t want to be editing anything.

Find the sketch that you want to move.  The sketch could be consumed by a feature…it doesn’t matter.  Then you can right mouse click on it.  This will cause the in-context property manager to appear.  The great thing is that it’s right next to your mouse.

You will want to choose the ‘Edit Sketch Plane’ option.  This allows you to move it to a different face or plane.  It is the icon that looks like a plane with a hand pointing to it.  It is the second icon.


You can also get to the option under Edit, Sketch Plane.  It’s the same feature as on the in context tool bar.

It then asks you where you want to place the sketch.  You can choose either a different face or a reference plane.  The face that you choose could be parallel to the original one, perpendicular, or angled.  It doesn’t matter where it is.

It is possible that you will get a message box that says something about moving it to a different face will cause dimensions or the relations to fail.  That happens when the edge you were originally referencing cannot be found.  I would suggest just choose to delete the item and add the dimension/relation back in.

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Save SolidWorks Assembly as a Part

 

It is a common practice to export a SolidWorks assembly to a neutral file format to be imported in other CAD applications.  The option to save SolidWorks assembly as a part may not be as widely used, but it can be useful when assembly file set needs to be reduced to a single file and used for representation only.  Saving assembly as a part eliminates the need for sending all the reference files.
To save an assembly as a part, we use the File > Save As command.

Save SolidWorks assembly as a part file

After .sldprt file type is selected, three options appear in the Save As dialog:

1. Exterior faces – saved part includes external faces only, all bodies being surfaces.  Typical reasons for saving assembly as a part with external faces are preventing reverse engineering of the model and reducing file size of the model that is required for representation purpose.
2. Exterior components – part includes only visible components.
3. All components – all components are included as multiple bodies except those that are hidden or suppressed in the assembly.

Similar to exporting assembly to a neutral file format, a part saved from an assembly includes plain geometry without feature history.  After an assembly has been saved to a part file, there is no link between the two documents.  Further changes made to the assembly will not propagate to the part file.

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Drawing Move View or BOM to a different Sheet

When a SOLIDWORKS drawing sheet becomes crowded and difficult to read, it may help to know that it is possible to move a drawing view or a BOM to a different sheet.  All dimensions and annotations move with the view.

Applying SOLIDWORKS Drawing Move View

In the design tree, activate the sheet that includes the drawing view that is being moved.  Click on the view with the left-mouse button and keep the button pressed.  Drag the view and hover over the name of the sheet to which it is being moved.  When the icon that looks like a yellow bent arrow pointing to the left appears, release the left mouse button to drop the view on the sheet.

Drag and drop a drawing view to a different sheet

The same method works for moving BOMs from one sheet to another.  The sheet that includes BOM must be active before the move.

Drag and drop a BOM to a different sheet

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Verification on rebuild (enable advanced body checking)

Controls the level of error checking when you create or modify features. For most applications, the default setting (cleared) is adequate and results in a faster rebuild of the model.

When you run a Ctrl+Q (forced rebuild), SolidWorks will rebuild your sessions edits. But a forced rebuild will not run a stringent check on bodies, faces and edges by default. When working with complex models and surfaces this check is paramount. Having this setting cleared can lead to disaster down the track, and the user in none the wiser.

This setting can be found at: Tools>Options>System Options>Performance>

Setting in SolidWorks under Tools>Options

By default this setting is off…
Reasons for having it off:

1.        SolidWorks rebuild time will be faster
2.        Sheetmetal flatten/un-flatten feature faster

Yes… only 2 reasons (and in my mind not good ones)
Reasons for having the setting enabled:

1. SolidWorks® preforms a stringent check on solids and surfaces ensuring that they are valid
2. Avoid unexplained geometry errors further down the feature tree
3. When creating drawings, ensures that you have high quality views
4. Exporting to DXF/DWG without error
5. Avoid zero thickness geometry being created
6. Unexplained transparencies on faces in a model
7. Avoid invalid surfaces
8. Ensure Scale feature can work
9. Ensuring correct mass properties calculation

The list can go on and on…
The biggest example that I’ve had on Support regarding this setting is when a customer called in saying he’s got a large assembly and he needs to get the parts exported to DXF for the suppliers asap but cannot, the DXF file is empty!

I noticed that upon opening the drawing files that needed to be exported to DXF, all the views were in draft quality. The problem boiled down to modelling without the verification on rebuild setting enabled. Once we enabled the verification on rebuild setting many part feature trees lit up like Christmas trees with red cherries all over them. The user was none the wiser for months modelling as SolidWorks was not reporting the errors due to not validating the validity of the surfaces and bodies in the models. Once we set a few models straight by fixing up the errors the drawing views now where in high quality and the DXF export worked!

Watch out for this setting, as in the case above the poor customer was up for weeks of repairing models, and he ended up submitting late to his supplier.

You may have heard in the past that this setting will slow you down. This is an old school way of thought; with the PC’s we have now this setting will not slow you down enough to worry.

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Image Quality Setting (Drawings)

The image quality setting in SolidWorks can be your friend or… your worst enemy:

With SolidWorks® drawings sometimes you can get issues like;

Edges on models show in some views but do not in other views
Dimensions not attaching to edges correctly
Incomplete printing
Parts missing
Incomplete section views
Export to DWG/DXF and PDF issues
File size issues
Zoom/pan performance
and many others…

The “Image Quality” setting in SolidWorks® found under Tools>Options>Document Properties>Image Quality

When the 2 image quality sliders are too low, you can have issues as mentioned above, also if the sliders are too high you can have issues with performance, as the file size will be much larger. If your drawing is a large drawing file moving these sliders down can help with performance. But when it comes time to print or export your drawing to a PDF say, jump in and move these sliders up to say %80. Going too high can lead to an unreasonable drawing file size.

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