Posts Tagged ‘drawings’

Weldments and Bill of Materials

Wednesday, March 26th, 2014

There are many different ways to create structural frames.  One method might be creating it as an assembly with many individual parts.  Another method, which is my preferred  way, would be as a single multibody part…as a Weldment.
Weldment Icon
The Weldment way allows for easy design changes, automatic structural member trimming/extensions, and creation of cut lengths.  This however is typically just a portion of the overall design.  There might be many more pieces that go on the frame.  This is when you would add your Weldment design to an assembly.

Now with your Weldment in the assembly and the other components attached, you need a Bill of Materials (BOM).  It’s possibly to show the cut list for all the structural members in an assembly BOM.  You will need to choose a BOM Type of Indented in the PropertyManager.

BOM Property Manager
Once you choose the indented type, the BOM will show as a cut list.  The QTY column shows a total length for the structural member.

BOM Image
If you then choose “Detailed cut list” in the BOM Type, it will break each member out in their own row with a length value.

BOM Image Detailed
Now your assembly BOMs can show all the individual items even in the Weldment.  But what if you are using Enterprise PDM.  Can you see the cut list in EPDM?  Of course you can.  It is under the Bill of Materials tab.  You would need to set-up a Weldment Cut List template in EPDM but that is very simple.

EPDM Cut List
As you can see, the cut list item names can be shown to make finding the correct member easy.  Just like in a drawing, you can choose to see a Weldment BOM.

EPDM Weldment BOM
This will group all the members together giving you a total quantity.  If you select the “Contains” tab, and RMB on a Weldment member, you get some more useful functionality.

EPDM Contains Tab
When you choose “Properties”, you can see the members data card with the length.

EPDM Data Card Weldment
You will need to add the length field to the card and map it to the “BOM Quantity” variable.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

Compare images and drawings

Wednesday, December 12th, 2012

Surprise, surprise.

You customer changed their design -again.

He just sent you a new set of drawings…aaaannnnd as typical, did not bother to send you a list of changes.

Now you need to check each dimension, one at a time, looking for who knows what kind of changes you just got stuck dealing with.

Actually, there is a good chance you can use SolidWorks’ DrawCompare to compare the files.

It is true that DrawCompare only compares SolidWorks drawings; there is nothing to say that you cannot turn your bitty brain customer’s files into SolidWorks drawings!

If the files you want to compare are jpg, bmp, tif, png, wmf, or psd files, create a new blank SolidWorks drawing (without a titleblock.) Insert the drawing as a picture and place the image on the origin. Then save the new SolidWorks drawing file. Do this for both files you want to compare.

[Your results will vary. I've found black and white images work best, the compare quality diminishes as you get more and more colors.]

If the file is a dwg/dxf file, open the file in SolidWorks and save it as a SolidWorks drawing file.

(use “Convert to SolidWorks entities” option, do not embed as a sheet) Ensure you use the exact same scale for both files, and ensure the entire file fits on the sheet format. Do this for both files you want to compare.

Now that you have two new “SolidWorks” drawings…in Solidworks, Tools -> Compare -> DrawCompare…navigate to the new files you created, and the tool will show you the differences!

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Auto Arrange Dimensions

Monday, May 21st, 2012

One of my favorite enhancements to drawings over the past couple of years has got to be Auto Arrange Dimensions. This might be as close as you get to an ‘easy’ button in drawings. See the image below to discover a drawing view with the dimensions in a complete mess.

To fix this in flash, SolidWorks introduced Auto Arrange Dimensions the the 2011 release. This function will automatically arrange the selected dimensions for you. The procedure is as follows:

  1. Box-select all of the dimensions.
  2. Next, move the mouse pointer over the Dimension Palette rollover button     to display the dimension palette. (Incidentally, if you mouse AWAY from the Dimension Palette rollover button, it will disappear. To get it back just hit the CTRL button on your keyboard.)
  3. On the Dimension Pallete, click Auto Arrange Dimensions in the lower left corner
  4. Click in the graphics area to turn off the Dimension Pallete – Easy!

When you use Auto Arrange Dimensions, the selected dimensions are placed as follows:

  • Spaced from smallest to largest
  • Aligned and centered, if possible
  • Spaced with the offset distances defined in Document Properties – Dimensions
  • Adjusted to avoid overlapping
  • Staggered, if necessary

There are a number of other tools on the Dimension Palette that you will also want to check out for when you have multiple dimensions selected and you want to make some adjustments – including Space Evenly Linear/Radial, Align Collinear, Align Stagger, Justify Text and Dimension Spacing Value (either numerical input or thumbwheel). Enjoy.

Chris Snider

Application Engineer, CSWE 3DVision Technologies

A Few Drawing Tips

Monday, September 26th, 2011

Here are a few drawing tips that might help you out.

Save a rotated 3D view

  • When you go to View>Modify>3D Drawing View, you can choose any view and rotate it any direction.  When you choose a view that you like, it will stay like that.  That way you can get a great view on the drawing with a short amount of time.

Combine notes

  • If you have multiple notes on your drawing but you want to combine them, before you would need to copy and paste the text.  All you really need to do is just drag and drop one note to another.  They get combined.  If the main note is numerically indented, when you drop the other note on it, it will follow the same order.

Edit multiple dimensions at once

  • If you select a bunch of dimensions, you can edit them all at once.  You can add tolerance information, text, precision, etc.

I hope these tips help keep you productive.  If you have any questions about these, please contact 3DVision.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

Update Properties from BOM

Monday, August 22nd, 2011

Here’s a tip that you might not know about.  You can update component/sub-assembly properties from a Bill of Materials.  Why would you want to do this?  Well in case you forgot to add the property when you created the component, maybe you didn’t know what it was at that time, or you see you filled out the wrong information.  Now you can add or change the property without opening it up.

All you need to do is double click in the cell of the BOM and then you will get a message about keeping or breaking the link.

Link

You will have to choose “Keep Link” to update the property.  Now whatever you type in the cell will show up in the component’s properties.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

Search for Dimensions in EPDM

Monday, July 25th, 2011

Great Aunt Eleanor can do many amazing things. She can name and describe all RAID configurations, she can rewire an HDMI connection so her old black and white movies will be black and white again (she curses Ted Turner the entire time) and apparently she is the lead elf in her WOW guild…but she can’t cook. The lady can [and has] burnt water. Thus apparently it would be logical for her to buy an Indian restaurant.

The nice thing about Indian dishes is that they are pretty easy. Every thing is brown, crazy spicy and all the food is cut up into simple hexahedrons. The only thing different about the hexahedrons is their length, width and height.

Great Aunt Eleanor has decided she wants to SolidWorks Enterprise PDM to be able to store her food cutting guides. She wants to be able to enter in a few dimensions in a search window and have EPDM return all the food pieces that meet the search criteria. This is her datacard:

Datacard

Pretty nice, though since Great Aunt Eleanor is always playing with the sizes, she wants to link the dimensions of her SolidWorks models to the datacard. So if the food size changes, the datacard updates automatically.

Here is how I linked her dimensions to the datacard values.

Dimensions

I created the three custom file properties (height, width, length), then for value, I used this format: “Dimension Name@Sketch Name@File Name”. I usually find it easier to click in the “Value/Text Expression” column and then click on the dimension. SolidWorks build the required format for you. (Note: the dimension names were renamed by me, typically they will have a “D1″, “D2″ type format.)

FileProperties

Now your file properties update as the dimensions update, all that is left is to connect your EPDM variables to your file properties, and thus as your model dimension change, your EPDM database updates automatically!

Next Great Aunt Eleanor stored this file as a SolidWorks template, so when she comes up with a new food type, (perhaps something brown-ier?) she starts with the template and the settings already to go.

Another tip, make the controls in the datacard read-only, that way they only way they are updated is via changing the SolidWorks model.

Now Great Aunt Eleanor can quickly use EPDM to search for the exact size of food she needs.

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

SolidWorks Sheet format

Monday, May 9th, 2011

Yesterday I caught Great Aunt Eleanor browsing on my computer. I hate it when she does that -she always finds a setting or something I am doing wrong and makes fun of me.

Yesterday was no exception.

“Why do you have so many SolidWorks drawing templates?” she queried.

I think I have her now, she thinks she is so smart. I explain to her that I need to have a drawing template for each sheet size (A, B, C, D, & E) and I need a template because sometimes I design in metric, sometimes in old people units. (I call inches “old people units” -’cause it gets under her skin a bit). “Five sheet size times two units equals ten files!” I say with a smug look on my face.

“What if you need to make a change to a SolidWorks option, or SolidWorks adds a new option that you want to incorporate into your templates? That’s ten files you need to update, ten times the setup, ten times for you to make a mistake. You should be using sheet formats. They make building your template library easier.” she replied shaking her cane at me, heading back to her computer muttering about mining more gold than some guy named Deathwing.

“’cause I don’t want to!” I shout. “Sheet formats are stupid!”

Okay, at this point I had no idea what a sheet format was, but I couldn’t let her know that.

Sheet formats (.slddrt) are actually very cool. They are really a simple file that contain only your titleblock. It is just a sketch with some properties.

Your SolidWorks document settings are stored in the .drwdot file. If you work in metric and imperial you’ll typically need only two of these files, one for each. Create five titleblocks [sheet formats] and you only have seven files to maintain rather than ten. If in the future, you need to make a change to a drawing setting, all you have to do is update the two .drwdot files -the sheet formats are only overlays.

I know this is a little confusing, so let me show you how to do it. First, open your drawing template, delete the sheet format

DeleteSheetFormat

go through and set all of the document properties

DocumentProperties

and save this file as a .drwdot file. Call it something like: “Old People Drawing”

Now, when you want to make a new drawing with your inch settings, Choose the “Old People Drawing” template. Since this template does not have a sheet format, SolidWorks will ask you to choose the sheet format you want to use:

sheetsize

All that is left is to make your sheet format.

Build your sheet format (typically just your titleblock and boarder) with your sketch tools and save it

SaveSheetFormat

in the same location where your sheet formats are located:

SheetFormats

Make a different sheet format for each drawing size or titleblock and you are good to go! Much easier to manage.

Another point to Great Aunt Eleanor.

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Improve your efficiency with Drawings

Wednesday, February 16th, 2011

One of the biggest pain points in SolidWorks is drawings.  It’s not that creating a drawing is difficult – far from it.  Creating multiple drawing views is as easy as dragging and dropping predefined views from the View Palette.

2011-0215a View Palette

I believe drawings are perceived as difficult due to the amount of time people spend trying to make their drawing “just right”.  As an Engineer or Designer you spend a lot of time creating your CAD models, adding dimensions and sketch relations, so you know exactly how each feature will behave.  Your investment is making your CAD model “just right”.  So why after placing a handful of drawing views onto your drawing sheet(s) are you manually recreating every dimension?  That is what Insert Model Items is for!

2011-0215b Insert Model Items

I’ll be the first to admit that using Insert Model Items is a scary proposition.  Dimensions often seem to propagate onto drawing views randomly.  Rather than cleaning up dimension placement, you manually recreate all of the model dimensions on the drawing.  I’m not one to recreate the wheel, so I’ll point you to a great blog article written by one of our friends at Javelin Technologies, Alin Vargatu, CSWE.

Do you want to save a lot of time when dimensioning your drawings?

Now that you’ve read about time saving methods for dimensioning drawings, you’ll have more time to improve upon the wheel. Good luck!

Bill Reuss

Elite Application Engineer CAE Technical Specialist 3DVision Technologies

Automatically Align Broken Views

Monday, January 17th, 2011

I like having things done automatically – except for shifting the transmission in my car and having funds removed from my bank account. In the world of SolidWorks Drawings, however, the more automatic, the better.

I recently discovered a little trick with broken views that I thought I would pass along. Ever want to line up the breaks on 2 broken views of the same part? If the second view is a projected view, you are in luck. The steps are easy – place the first view (e.g. Front) and create the broken view on that view. Once you get it how you like it, use the Projected View command to create the second view and the Broken View comes along for the ride – automatically aligning the gap in the Projected View with the original view.

See the image below for details.

 

Broken view

Chris Snider

Application Engineer, CSWE 3DVision Technologies

Keep Balloon Numbering Consistent

Wednesday, January 12th, 2011

Recently, I received a call from a customer in Columbus, OH, that designs and manufactures a variety of sheetmetal components for shelving and fixtures.  As you can imagine, a complex shelving design may require several drawing sheets to adequately describe the product to the shop floor.  The Shop wanted the Engineer to maintain balloon part numbering from the first drawing sheet to the last drawing sheet.  Personally, I don’t blame the Shop for wanting their information as clean and concise as the Office personnel – they already learned about stable item numbering in Enterprise PDM several months ago.

Sheet1 is an assembly drawing with an Indented Bill of Materials using the Flat Numbering option.  I’ve added the balloons for two components that make up one of the sub-assemblies for a pressure vessel.  The Shop wants the Engineer to create drawings where the numbers are consistent, regardless of the drawing sheet.  For the example, balloons 26 and 27 need to identify the same component on all drawing sheets.

Drawing Sheet1, Indented BOM, Flat Numbering

Sheet2, shows the sub-assembly that includes components 26 and 27 from Sheet1.  With a simple RMB in the drawing view, select Properties.  This brings up the Drawing View Properties dialog.  Check the box for ‘Link balloon text to specified table’ and then select ‘Bill of Materials1′, which is on Sheet1 of our drawing, the balloon numbering on Sheet2 matches Sheet1.

Sheet2

Give it a try the next time the Shop complains about your drawings and balloon numbering!

Bill Reuss

Elite Application Engineer CAE Technical Specialist 3DVision Technologies

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