Graphics Systems SolidNotes

SolidWorks Tutorial: How to Get Colored Crosshatch in Section View

There have been times when I wanted to show a section view with the crosshatch in a different color than the default black. Here is what the default view looks like.

Here are the steps to get a different color for the crosshatch.

• Create a new layer and give it the color, line style, and line thickness you want.

• Select the default crosshatched area on the section view.
• In the Area Hatch/Fill Property Manager, uncheck the “Material crosshatch” checkbox.

• Then select “None” as the option for type and select “OK” (green checkmark).

• Select the area (or areas) that you want to have crosshatched.
• Go to the Insert dropdown menu and select “Annotations > Area Hatch/Fill”.
• Here is where you can select what style of Hatch you want to have on the area.
• Then select the newly created layer (color layer).

• This is what your colored drawing view will look like.

 

How to Change Company Logo on SolidWorks Drawings

Has your company updated their logo? Is the company logo in all your drawing title blocks? How do you update that logo on all your drawings?

There are two ways to accomplish this depending on if your original objects are linked to an external file:

Option 1: If the Original Object is Not Linked to an External File--

• Create the new image file of the company logo in an image editing program. Hopefully, there is a file that is close to what you need and you can modify that.
  • As a note, it is best to make the size of this image file be the size you want it when it is inserted into the drawing template (for example, 2 inch by 2 inch). This means that after you insert the image, you do not need to grab the image and scale it at all inside SolidWorks.
• Open your drawing template file and insert the new logo. To do this, click on Insert=>Object. When the following window opens, select “create from file” then browse to your new logo file. Then check the “Link” box to make sure the drawing template is connected to the original file. Place the new logo where needed.

                          

•  
  • Just as a note, this means that the original image file needs to stay in the folder selected. If the image file has been deleted or moved, the image that shows on the drawing will be what was last saved (not necessarily the correct one). I suggest that the image file is placed somewhere on the network that everyone has access to because any user that opens the drawing template needs to be able to access the image file.
• Save the drawing template file and the sheet format file with the linked image file.
• Open each drawing file that exists and manually change out the image file with the new logo image file. Yes, every drawing file that exists will need to be opened, modified, and then resaved.

Option 2: If the Object is Already Linked to an External File--

• Modify the image file that is saved on the network as the drawing template logo file.
  • Make sure that the size of the logo is the same as the original. This will insure that when the new image file is automatically updated in the drawing, the size of the image on the drawing will not change (and possibility move or cover some other text or line on the drawing template).
• Have SolidWorks Task Scheduler update all drawings automatically. Or, when you open the drawing it will automatically update the image file. Then, when you save the drawing, it will have the new company logo (you do not need to manually change anything).

 

New SolidWorks 2013 Function: Convert Drawing View to Sketch

Have you ever wanted to take a drawing view and make it into a standard block that you could use in layout drawings? You have a part model, but you only want a 2D “picture” of it? SolidWorks 2013 has a new command that makes this a breeze!

Simply right click on any model drawing view and choose Convert View to Sketch.

 

If you want to define a sketch block, choose that option and set the insertion point as you would any other block you create in SolidWorks.

 

Click to place the block and viola! There’s your block.

Linking a Bill of Materials To a View in SolidWorks

Linking a BOM to a View (on a drawing) is accomplished by the following:

• Click the right mouse button on the view
• On the pop up menu choose properties
• In the Drawing View Properties Dialogue box check Link balloon text to specified table
• Choose the correct table (BOM) from the drop down below.

 

This Process will resolve or answer the following questions and issues:

Why does the balloon numbering not respect the bill of materials (BOM) item numbers?

        This can occur for drawings where multiple bills of materials (BOM) were previously inserted or are         inserted.

 Why does a balloon attached to a general view get a number not listed in the bill of materials?

    When attaching a balloon to a component in a view (different from the view used to create the bill of     materials), the balloon automatically gets the number, following the FeatureManager® tree of the     configuration specified in the view.

Is it possible to link a balloon attached to a drawing view of a part to a bill of materials (BOM) of an assembly that contains that part?

    Yes, it is possible by specifying the BOM which the drawing view/balloon is looking at and using the     drawing view option ‘Link balloon text to specified table’. This is valid if the BOM is contained in a     different sheet as well as in the same sheet of the part drawing view.

Why are the balloons in a drawing not following the Bill of Materials (BOM) numbering?

    The balloons in a drawing may not be following the Bill of Materials if the drawing view is not linked to     the BOM and therefore the balloon numbers are defaulting to assembly order.  In order to link drawings     view to a check the box for "Keep Linked to BOM."  In the pull down menu select the BOM name to     which to link the drawing view.  The balloons added to the drawing view will now match the BOM item     numbers.

If creating views from parts on an assembly drawing all the balloons attached to the views display the number “1”. Is it possible to get the correct balloon number from the assembly drawing view/ bill of materials (BOM) table?

    This is possible using the option ‘Link balloon text to specific BOM table’.

    Check the option ‘Link balloon text to specific BOM table’ and chose the specific BOM table to apply
    The balloon will get the number from the BOM.

Show Part as “See Through” using Alternate Position Function in SolidWorks

Have you ever had an assembly that uses a component that you didn’t want to show in the BOM but you still wanted to see it in the drawing view as “see through”? The most common use for this that I can think of is showing a part that is being held in place by a fixture. You need to have the fixture components in the BOM, but you do not want to show the part. However, on the drawing views you want to show the part for orientation purposes.

By utilizing the Alternate Position function, you can show your part as “see through” and not have it included in the BOM.

To accomplish this, first create your assembly with the part in it (this is automatically the Default configuration). Then create a configuration called “Part Not Visible” (or something similar). Suppress the part in the Part Not Visible configuration.

In a drawing, create a drawing view using the Part Not Visible configuration. 

Select the newly created view and then go to Insert=>Drawing View=>Alternate Position.

In the PropertyManager window, select “Existing configuration” and select the Default configuration.

Your drawing view now has the “Part” shown as phantom lines but “see through”

Now, when you create a BOM from this view, the “Part” will not be in the BOM (just make sure the BOM is referencing the Part Not Visible configuration).

 

 

SolidWorks, The Basics: Saving Sketch Dimensioning Styles

Can you imagine doing your job without the benefits of a top-flight 3D modeler like SolidWorks? I thought not. I am sure you remember the excitement you felt when you learned the power of the tool at your disposal. And the education didn’t stop there, did it? To this day, you enjoy learning new things. That’s why you’re reading the SolidNotes blog, right?  

However, here’s something I have long noticed: In my interactions with users, even very experienced ones, a lot of the questions involve seemingly basic procedures. I think it is easy to jump into the deep end and gloss over many such seemingly routine operations. Hence, another topic in my Basics Series: Sketch Dimension Styles.

We are often taught, when adding dimensions in a part sketch environment, to not worry about stylistic options or even exact unit precision or tolerances. That information can come later, on the drawing. That is often sufficient and is not incorrect. However, there are options that let you better tailor your dimensions in the sketch environment and can be instrumental in capturing intent and reducing errors downstream.

Fig. 1

Figure 1 shows the Sketch Dimension Property Manager. On the Value tab, we see a Tolerance/Precision node, under which I have selected Symmetric from among the many choices. Below that are pull-down menus that allow me to control the number of place precision of the dimension and its tolerance, and I have entered those tolerances accordingly.  

As this is something I plan to do with some frequency, I have chosen the “Add or Update a Style” and entered “3 PL” for a style name in the ensuing dialog box. I now have a named style that I may select to be current or use to change that of an existing dimension. As you might expect, these dimensions will keep these appearances when displayed in your drawing.

And…why, yes!   This *is* something I can create and save in my part template!  Similarly, this can also be saved as a style (“.sldstl” file format) and opened from another document, such as my drawing template, with the Load Style button.

 

A Minor Annoyance—Solved

We’ve all been there: we make a section view or detail view in a drawing, decide we don’t like it, then delete it. Then we try again, and the label for the new drawing view has advanced. We change the label, then go to the Sheet Properties and reset the count back to make sure the next one is correct—at least until the next time we delete a labeled view!

SolidWorks 2012 has a solution: in the System Options, on the Drawings page, near the bottom of that long list of checkboxes, you’ll see an option to “Reuse view letters from deleted auxiliary, detail, and section views.”

 

 

Simply activate this switch and viola! SolidWorks won’t advance the view label when you delete your next section view; instead, it will use the label from the deleted view again for you new section view.

I love it when I find a little nugget like that in the options, don’t you?

Want to Hide those Internal Notes on your Drawing?

Everyone outsources jobs to vendors these days and many times you write notes on your drawings that are intended to stay internal. On occasion, we need to be able to hide those internal notes before sending it outside. SolidWorks has a great way to control those internal notes through using an option called empty view. This is a little secret that if you took the drawings class you probably already know this tip. If not, here's what you do:

    1) Insert, drawing view, empty.

    2) Place empty view on the drawing.

    3) Lock view focus on the empty view as to ensure that you are working on the correct view.

    4) When you want to hide those secret internal notes you simply right click on the view in the feature     manager design tree. This method of hiding notes can become a company best practice. Enjoy…

Twenty Years, Sci-Fi and eDrawings for iPad

Today marks my 20th anniversary at Graphics Systems Corporation. Originally, I was going to blog about how engineering and design technology has changed. You know:

• 2D CAD that used to cost $4000 is now freely available at no charge
• 3D CAD that used to require heavy, specialized hardware and cost $30,000 now runs on laptop computers, costs less than $4000, and does more
• Simulation that used to take days to set up and run can now be completed in minutes, while enjoying the same economies of cost and standard hardware as 3D CAD
• Data management that took years to implement, cost well into the six-figure range and was too complex for most people to use can now can be implemented in weeks, at a fraction of the cost, and can be used by anyone
• Tools now exist to allow the direct reuse of 3D CAD data for manufacturing, marketing, and technical publications professions, eliminating the manual recreation of data that used to be necessary for those functions.

It turns out, however, something far more exciting happened today in the SolidWorks community than my 20th anniversary in the MCAD industry. Today, we can begin to mimic Scotty and Geordi and carry our engineering data in the palm of our hands, for today eDrawings for iPad has been released.

This is an incredibly important step in the development of the SolidWorks ecosystem. eDrawings for iPad is an excellent tool, and this first effort has enough functionality to make it very useful on the shop floor, in the conference room, and in the field. File access is available through traditional iTunes file transfer and services such as Dropbox; however, there are already iPad clients for ePDM that allow raster preview of data, so I would expect at some point in the future these two technologies will get together. That's not any inside information, that's just me making an easy prediction.

Twenty years from now, we'll be doing design on touch devices and our data will be instantaneously accessible from anywhere on the planet. Actually, that will probably happen in half that time. Maybe in twenty years we'll be doing better than that -- think about the interface between Tony Stark and Jarvis.

(What? You've never seen Iron Man, and you're reading this blog? You need to Netflix/iTunes/Redbox/on-demand it, because as much as anything, it's a movie about the future of design and manufacturing. Notice how I didn't say "go out and rent it"? Yeah, we're in a bit of the future right now...)

So, here's to twenty great years of computer-aided design, engineering and manufacturing evolution. Hit me back in 2032 with whatever technology we'll be using, and I'll do a follow-up.

Oh, did you want more about eDrawings for iPad? Try here to read about it and see a video of it in action, and here to download it from the Apple App Store (it'll cost you a whopping $1.99). If you want to get your own files into the app, you can use any file-access app (like Dropbox) and "Open With..." to bring it into the eDrawings app. It works by displaying the graphics for native SolidWorks files, so you don't need to upload all the parts to go along with an assembly, unless you want to view the parts individually. That's pretty much all the training you're gonna need -- download it, play with it and use it.

How To Create Multi-Line Custom Property Values

Did you ever want to have a custom property value show up as two or more defined lines of text? In most Windows text-handling applications, you use a "forced carriage return" by typing <CTRL>ENTER at the end of the line. Like this:

Two
Line

There is a simple way you can use this in your custom property values. Just type the text, as you would like, in a simple text application like Notepad:

Next, highlight the two lines of text (all together as one selection, to insure you pick up the invisible CTRL-ENTER "character") and Copy it to the Windows clipboard:

Then, switch to your SolidWorks custom property dialog, and paste the result into the appropriate Value / Text Expression box. When you do this, you'll only see the first line show up in the Value / Text Expression box, and you'll only see the last line show up in the Evaluated Value box. All the text is there, however -- it just can't all be displayed in the single-row-high text boxes in the dialog:

When you reference the property value somewhere else, such as a drawing title block, you'll see all the lines of text are there, with the line breaks you specified.

This is something my brother John and I figured out many years ago during one of our live SolidWorkout sessions. It's came up recently with a customer -- and it's still useful -- so I thought I'd share it.

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