Posts Tagged ‘drawings’

Multi-language in Enterprise PDM

Tuesday, January 27th, 2015

In SOLIDWORKS Enterprise PDM, I do not like the idea of mixing languages within the same Enterprise variable. I want to be able to run reports and see BOMs in a chosen language.  Multi-language reports and BOMs are difficult for users. I like adding a suffix to each variable name for each language, i.e. “Finish” is broken in to multiple languages: “Finish-English”, “Finish-French”, etc… Then define different BOM column sets pointing to each corresponding language.

BOMListFinishes

Same concept for search cards, reports, file properties, etc.

It is difficult to have one title block support multiple languages/business units. Beyond the fact that the block needs to be bigger to support multi-languages, each group likes to have their address, phone number, logo, etc.  Usually it is easier for each language to have its own sheet format with fields pointing to the proper language’s file property. It only takes a few seconds to swap sheet formats in drawings. (It may be a slightly modified macro that swaps the language specific notes?)

Some company’s default sheet formats are only a rough skeleton showing designers their drawing area, the proper “language appropriate” sheet format is only applied when needed -printing. (Since meta data is just to the right of the drawing preview in the viewer, internally a title block may not have much value.)

In summary: The part file has a file property for each language it needs to support. The drawing sheet format points only to the property of the language it needs. Swap the sheet format, the new title block is now in the new language.

The downside to all of this is that you need to collect data in multiple languages and your data cards need to support this. If your users don’t speak all the languages your files require, you can either have the second language group populate the data cards as needed, or give your users cross reference look-up tables so they can populate the entire data card themselves without needing to know how to speak the other languages. 3rd party tools such as PigeonHole can help you do this:

YouTube Preview Image

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Changing languages on drawings

Tuesday, January 6th, 2015

I know companies that spend a lot of money translating drawings. Typically it is a slow, tedious, manual process. Since often times the translators aren’t engineers, you can sometimes get embarrassing translations.

If your standard notes are blocks, translating these notes can be done very quickly.

SOLIDWORKS’ blocks have a “FileName” property that a macro can easily change. Change the “FileName” property and the block immediately changes to the new block. So if you are clever about your block naming strategy, a small macro can be used to quickly change your notes from one language to another.

I break my notes in folders by language:

DesignLibrary2

For example above I have three “Chamfer.sldblk” files. All with the same file name but defined with different languages as the text within the block.

The English version is in: “c:\vaultname\Standard Notes\English\Chamfer.sldblk
The French version is in: “c:\vaultname\Standard Notes\French\Chamfer.sldblk
The Mandarin version is in: “c:\vaultname\Standard Notes\Mandarin\Chamfer.sldblk

This little SOLIDWORKS macro snip cycles through all of the notes in a drawing, looks at their path, if it finds the word “English” in the block’s file path, the block gets changed to the “French” version.

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim vBlockDef As Variant
Dim SwSketchMgr As SldWorks.SketchManager
Dim swBlockDef As SldWorks.SketchBlockDefinition
Set swApp = CreateObject("SldWorks.Application")
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
Set SwSketchMgr = swModel.SketchManager
vBlockDef = SwSketchMgr.GetSketchBlockDefinitions
If Not IsEmpty(vBlockDef) Then
For i = 0 To UBound(vBlockDef)
Set swBlockDef = vBlockDef(i)
swBlockDef.FileName = Replace(swBlockDef.FileName, "English", "French")
Next i
End If

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Store common notes as blocks

Monday, January 5th, 2015

A library of drawing notes for your drawings:

  • Helps save time
  • Avoid confusion with groups outside of engineering
  • Makes training easier for new hires
  • Make things easier if in the future you need to make changes to your notes through automation.

I like turning my common annotations (notes) into blocks, then saving the blocks into my design library.

DesignLibrary2

Now when I am ready to add common notes to my drawings, I can drag and drop my notes from the SOLIDWORKS task pane to where I want within the drawing.

If you store these blocks in a common location where everyone has read access, everyone can take advantage of the standards you created.

 

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

Have you “Inspected” SolidWorks Inspection yet?

Wednesday, May 28th, 2014

SOLIDWORKS released SOLIDWORKS Inspection just over a month ago, so have you looked at it?  If you need to do any type of manufacturing validation and create inspection sheets for First Article Inspection then you should be using this tool. InspectionIcon

SOLIDWORKS Inspection has 2 versions: Standard and Professional.  If you want the ability to import CMM data or manually enter measured values to keep everything in one project then Professional is the version you need. INPro

Every license of Inspection comes with a stand-alone application and an add-in to SOLIDWORKS.  The stand-alone application allows you to leverage your legacy PDFs and TIFFs while the add-in uses the 2D SOLIDWORKS drawing. The add-in places the balloons directly on the SOLIDWORKS drawing giving the user full control of the shape and the look.  The dimension information is captured and the user has the ability to add other properties per dimension. INAddin

The stand-alone application uses Optical Character Recognition (OCR) to read the nominal dimension and tolerance.  This helps reduce typing errors from manual input. INStandOCR

With either application, you have the ability to output the inspection report as a user-customizable excel file.  This can easily be customized via the Inspection Wizard giving you great flexibility. INReport Click Here to visit 3DVision’s website for more information and to request a demo of SOLIDWORKS Inspection.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

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

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