CATI Tech Notes

SolidWorks Sheet Metal and Flat Pattern View Direction

One of the questions that came out of one of our training classes today is “How does SolidWorks determine the direction of the view layout for the Flat Pattern view it automatically generates?”

So we started looking and trying out different options and here is what we found, prior to SolidWorks 2011 we were unable to specify a Grain Direction in a sheet metal part so the Fixed Face viewed Normal To was the direction for your Flat Pattern. With SolidWorks 2011 SolidWorks added a series of new properties for Sheet Metal parts that a lot of information that is useful for manufacturing. Two of the Properties are Bounding Box Length and Bounding Box Width and because of this SolidWorks now lines up your Flat Pattern view with the Length in the Y and your Width in the X directions, thus for many people not give them the desired view layout. So if you want to change this you can use the Grain Direction, found by editing the Flat Pattern feature, and selecting an edge or sketch line for the Grain Direction (X).

The alternative option is:

1. Select the view to rotate.
2. Select the Rotate View icon found in the Heads-Up Toolbar.
3. Enter the value of the rotation angle.

Sheetmetal/Wood Products DXF Workaround

I had a customer looking to streamline the process of outputting DXF files to the shop floor with minimal work. This is what we came up with..

 

 

Hope you can use something like this....

 

See you at Solidworks World!

 

Todd Werginz

Technical Analyst

Computer Aided Technology

Changing Component Line Fonts

Not sure where you might see fit to use this, maybe it's been activated accidentally and you want to turn it off... but how?

Well if you wanted to change the font of a drawing view of a component maybe for a tech pub showing where component would be might be useful and selecting every line in the component seems like a waste then I have good news for you. There are 2 other options.

1) navigate to your drawing Feature Manager Design Tree, drill down to the view, and then to the component to change, and right click the component. Choose Component Line Font.

Here you have many options available.

You could also turn on the Line Format toolbar by right clicking the Command Manager ribbon and select Line Format. Then go to the Feature Manager Design Tree, drill down to the component, select it, then launch the Layer tool from the Line Format toolbar, then click the new layer and the Move button.

Happy holidays,
John Van Engen
CATI Tech Support

Custom Broken-out Section Views

Sometimes you may want to show a broken out section view in a drawing to see the inside of an assembly.  The broken-out section view tool that you have in the view layout tab can be difficult to control and doesn’t show well in an isometric orientation.  This can easily be done by creating an assembly feature cut.

I this case, I want to see the inside of the grill…

First create a sketch where you would like the cutout:

 

When you create the assembly cut, you have the ability pick and choose the components to be cut by using the feature scope.

 

Final results:

 

Now you can see the steaks cooking on the grill…

Enjoy,

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

Watermark Work Around

To trick SW into printing drawings with a watermark you need to use the following work around steps

1. Open a new or existing drawing file
2. Right click on the drawing sheet and select –Edit Sheet Format--
3. Now that you can edit the sheet format you want to insert a MS Word Document. Do this by going to –Insert -- Object –
4. In the Insert Object panel check -Create New- and select -Microsoft Office Word Document- as the Object Type. Click –Ok-- This will insert a MS Word Document into your SW drawing sheet format.

 
5. Now size the MS Word Doc to your specifications and go to the -Page Layout- tab and select  -Watermark -  Custom Watermark-

 

6. In the Custom Watermark Panel Select -Picture Watermark- and select the picture you would like to utilize. Click –ok-

 

7. Tada!! This will insert the watermark into the MS Word Document that is now part of your sheet format.

 

8. Finally click outside the MS Word Document to exit it and then right click and select –Edit Sheet- to exit the Edit Sheet Format mode and return to your drawing.

Note: The watermark will appear to be in front of any drawings inserted into the drawing sheet. However when the drawing is printed the watermark will appear as a watermark in the background.

 

Nick Jansen

CATI Technical Support

BOMs and Assembly Drawings

With the release of SolidWorks 2010, SolidWorks added some neat features when working with assembly drawings and BOMs.  First off, you will notice that when you select the BOM it now has a big, move icon that is now much easier to grab and move the BOM around.  The best of the bunch is the ability to move the BOM to a second sheet.  They have also added some nice visual cues to it…

When you select a component out of the view, it will highlight in the BOM.

 
Vice versa.  When you select the line item in the BOM, it will highlight the component in the assembly view. 

 

Grabbing the upper left hand move handle, you can drag the BOM to separate sheets (note: the sheet must be created first in order to drop the BOM on the sheet). 

 

And now that you have the part on a different sheet, it may be hard to remember what exactly the part looks like.  If you expand the triple arrow on the left hand side, you can now hover over the line item to see exactly what part it is your working with without having to toggle back over to other sheets.

 

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

 

 

Hiding bodies in a drawing view.

I ran into a call today that I haven’t seen in a while.  So, I’d thought I’d share…

Most people know how to hide a body in a multi-bodied part to focus or work on certain aspects of their design.  But, what about a drawing?  How do you hide a body in a drawing view?  The answer is quite simple:  Right-click on the drawing view and select properties.  A dialog box will open up like you see below.  Select the “Hide/Show Bodies” tab and select what bodies you want to hide out of the view.  Select “Apply” and “OK” to accept the changes.  And you’re done.  This same process can be used to hide components in an assembly.

 

 

Nathan Brunner, CSWP

Technical Analyst

Computer Aided Technology, Inc.

 

ISOMETRIC BROKEN OUT SECTION WITH CROP

        I had a question come up the other day with a cropped view. The customer was asking for a broken out section, (which BTW is an Awesome feature in Solidworks!) He had already cropped the view because it was a 95' long part and that did not look to good on the sheet. He was looking to get inside and show off
some of the componentry in the detail if you will. The problem is that this a current limitation in an Isometric view. So how do you work around this you ask???? Well I came up with this- in the assembly you can do a spline on a plane normal to the view you want to cut.

        I created a configuration at the assembly level called cutaway and sketched a spline at the assembly level.  I was able to control which parts it affected and if I wanted it to propagate back to parts. (No not really)

            So in the view it ends up looking like this after picking the correct configuration. All that is left is to use the break command from the View Layout toolbar on the command manager.

 

 

 

 

 

 

 

 

 

 

 

 

 

Todd Werginz, Technical Analyst

CATI

How to Show Sheet Metal Bend Lines in a Drawing

A customer had recently called in looking for a way to show his Bend Lines on the drawing of his sheet metal parts and while some people may say the answer is simple there are several ways to get the Bend Lines to show or not show in your drawing.

The first thing that everyone needs to know is where the Bend Lines are stored/create/saved, or whatever you want to call it. So in a part generated with the Sheet Metal Tools your Bend Lines are stored in the Flat-Pattern feature, remember that this sketch you can show/hide and suppress/unsuppress to control how/when it is displayed. By default it is always in the Folded configuration unsuppressed and hidden and in the Flat configuration it is unsuppressed and set to shown.

 

If your part was created in the “old school” method of Sheet Metal (Create features, Insert Bends). Your Bend Lines are stored in the same location as above but there are 2 other Sheet Metal Features that can interfere if you change the default way those are displayed, if you do not change anything with in them then you should have nothing to worry about.  

 

 

On to the drawing side of things, by default when you insert a Flat Pattern View from the View Palette or from the Model View command it will auto generate a derived configuration in the part file for you and drop in your Flattened view with Bend Notes.

 

If your view does not display properly then here is what you want to look at:

1. No Bend Lines but Bend Notes are show, then your Sketches are more than likely not set to View. Go to the View Drop Down Menu or the View Heads Up Menu and select Sketches.
    
    
2. No Bend Lines or Bend Notes are show, then your Bend Line Sketch for that view is more than likely not set to Show. Go to the Feature Tree and expand the View and drill down to the Bend Line Sketch, Right Click on it and set it to Show. You will probably be missing the Bend Notes and if you want those displayed Right Click on/in the View select Properties and Set the Bend Notes check box to show.
       
3. The last issue that we see is too many lines shown in the Flat and that is because in Part File someone has done an Edit Feature on the Flat Pattern feature and Unchecked the Merge faces check box. By un-checking this you well now see the start/stop of each face.
    
   Note: The Edit Feature of the Flat Pattern is also the area where you can change the Grain Direction of the part and for more information on this see the blog article by Jim Krivoshein, http://blog.cati.com/2011/02/sheet-metal-grain-direction-coil-direction.html

Josh Altergott

CATI Support Team Leader

Error Saving Sketches to Neutral File Formats

In working support calls yesterday I ran into a issue that could easily get anyone stumped, a customer had a file open that had a 3D Sketch in it and when they tried to save it out as a STEP, IGES or and other format they got an error that the data could not be exported.

The answer to this was actually pretty simple and the file that had the 3D Sketch in it was an Assembly file so I had the customer do the following:

1. Make sure you were out of Edit Sketch Mode in the assembly.
2. Start a New Part file and tile the windows so you can see both the part and the assembly.
3. Select the Sketch(s) from the Feature Tree of the Assembly and Copy (ctrl C).
4. Select in the Part file to make it active and Paste (ctrl V).
5. Perform a Save As, select your file type of choice. Note: Make sure to go to the options and set the options so that Sketches will export.

If you want to test the file before you send it on to whoever needs the information just Open that file into SolidWorks and see how it imports.

In the case of this customer they needed it so they could import this into MicroStation and they tested it in both SolidWorks and MicroStation while I had them on the phone and it imported just what they needed in both programs.

Happy Friday,

Josh Altergott

Support Team Leader