Posts Tagged ‘drawings’

DriveWorks for Sheet Scales

Friday, June 5th, 2015

If the overall size of your models change significantly, there is a good chance you will need DriveWorks to change your drawing sheet scales to keep your model looking nice on the sheet.

Imagine this is my drawing. Let’s say the height of my part does not change much, but my length (which is currently 100 in the model master) can change significantly.

DriveWorks Drawing


DriveWorks (Pro and Solo) gives us two sheet properties that we can use to drive the sheet scale:


If your company does not have standards on view scale requirements, the value of these two properties is rather simple. Set the numerator to always equal 1 and the denominator is a ratio of the new length to the old length times the current master sheet scale. So if my current sheet scale (in this example) is 1:5, my denominator rule would be (New length)/100*5. Making your rules look something like this:


Now your drawing will automatically scale up or down depending on the length of the part. (Make sure your views are all using the sheet scale Drive Works sheetscale…or you can create rules for the individual views too.) Granted, it makes for some non-traditional sheet scale values (My drafting teacher would die if I put “1:3.76″ on in the title block, I usually just put “NOT TO SCALE”) but nobody puts calipers on drawings anymore anyway.


…but what if your company is still using old standards that demand scales such as these:

Full size: 1:1
Enlargement scales: 2:1, 5:1, 10:1, 20:1, 50:1
Reduction scales: 1:2, 1:5, 1:10, 1:20, 1:50, 1:100, 1:200, 1:500, 1:1000, 1:2000, 1:5000, 1:10000

First, try to get an exception. (Why would DriveWorks created drawings have to follow this antiquated rule?) If you can’t get an exception, make a lookup table in DriveWorks.

DriveWorks Factors

Call the table something clever like “ScaleFactors”

First lets look at times when we want a reduction scale. (The numerator = 1). In these cases, we usually “round up” our numerator to the next larger scale factor (it is better for the views to be too small rather than being too big -and go off the page)

Now my previous denominator rule would look like this:

DMin(DwLookupScaleFactors,1,">=" & (New length)/100*5)

“DwLookUpScaleFactors” is the name of my table, I’m looking in the first column of that table, then finding the smallest number (DMin) that is greater or equal to the scale ratio that I calculated earlier. (So if my length is 100, DMin returns 5. If my length is 101, DMin returns 10)

In cases where we need an enlargement scale, the logic is the same except the denominator is = 1 and the numerator rule looks very much like the denominator rule above except you need to take the inverse of the ratio.

If you sometimes have a enlargement scale and sometimes have a reduction scale, an if/then statement is all you need. In pseudo code your denominator would say:

if("Enlargement scale",DMin(DwLookupScaleFactors,1,">=" & (New length)/100*5),1)

and your numerator would be

if("Enlargement scale",1,DMin(DwLookupScaleFactors,1,">=" & 100/(New length*5)) (Notice I took the inverse of the ratio)

Not very hard, but see why I wanted you to get rid of the scale factor standard?!

Questions about Driveworks or drawing sheet scales? Use the comment section below.

Jeff Sweeney

CSWE Engineering Data Specialist 3DVision Technologies

DimXpert Tips

Thursday, April 30th, 2015

With SOLIDWORKS MBD being released, you might be trying out DimXpert for the first time.  If you want to learn more about SOLIDWORKS MBD, check out my previous blog entry.  Here are some quick tips that might help.

Change Annotation Plane

When you have an annotation, you might need it to be placed on a different plane.  An example would be the dimension is on the TOP plane and you need it on the FRONT plane.  If you select the annotation, click the Single Quote button on your keyboard.  It’s the button with the ~ & `.


This will bring up the annotation plane box allowing you to choose where to place it.

Annotation Plane

Combine Dimensions

If you have multiple DimXpert dimensions and they are the same, you can combine them.  Just select them and RMB; it will give you the option to Combine Dimension.

Combine Dimension

Dimension Names

In the DimXpert Manager, the dimensions are just listed out with a generic name (i.e. Diameter1, Diameter2, etc).  You have the ability to rename them to whatever you want.  This can help with finding specific dimensions later.


Basic Dimensions

When you have a Geometric Tolerance, you might want to display the basic dimensions (the ones with a box around them).  If you select the GT in the tree, RMB and choose to Recreate basic dim.

Basic Dimension

Imported Models

DimXpert isn’t only for SOLIDWORKS files.  You can import other 3D models and apply dimensions to it.  The dimensions do not look at features but rather geometry.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

SOLIDWORKS Model-Based Definition (MBD) Has Been Released

Monday, March 9th, 2015

With SOLIDWORKS 2015 SP2, MBD was released at the same time.  Well what is MBD?  It is an integrated drawingless manufacturing solution.  Instead of creating a typical 2D drawing, all of the needed information is placed on the 3D model.  This helps reduce errors, increases production efficiency, and support industry standards.

You might wonder how this increases production efficiency.  It will make your process more efficient because there is not a need for 2D drawing files.  All of the information is already on the 3D file so why not use it?  The point of a 2D drawing file was to communicate to manufacturing on what the final item should look like.  This has been the main delivery.  A majority of the time it took to create the 2D drawing is now saved.


So you might be thinking that I still need to have dimensions and add notes so that will take a bunch of time.  All the time I am saving from the 2D drawing is being placed on the 3D model.  That’s not the case and leads me into the reduction of errors.  SOLIDWORKS MBD uses a tool that has been in SOLIDWORKS since 2008; DimXpert.  DimXpert is extremely powerful in creating PMI.  It has the ability to automatically create the manufacturing dimensions with tolerance on the 3D model.


But the reduction of errors comes with the ability to check all the faces for a dimension and tolerance by changing the face color.

SOLIDWORKS MBD’s main job is to organize all of the PMI data.  It does this by creating custom views to represent specific dimensions.  With 2D drawings you have multiple views with specific dimensions.  You do the same process with MBD by creating custom 3D views.  The helps deliver the intended information to production with less confusion.


How is the information delivered to production?  You have 2 options which are industry standards.  You can save the information to eDrawings or a 3D PDF.  The 3D PDF is fully customizable to match your requirements.


I feel MBD is a great way to save time, reduce errors, and communicate easier with manufacturing.  If you would like more information or would like to see a demo, please contact 3DVision @ 1-800-745-3136 or click here.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

Available Tables in SOLIDWORKS Drawings

Friday, February 13th, 2015

I get asked about the different tables in SOLIDWORKS drawings.  I’ll go over some of these as a high level overview.  This will cover BOM, Hole Table, Revision Tables, Weldment Cut List Tables, General Table, Weld Table, Bend Table, and Punch Tables.

Closed Table Rendered in SOLIDWORKS Drawings

The Bill of Materials is a list of the components and the quantities of each needed to manufacture the end product.  This can be customized a lot to be able to show different properties, different fonts, etc.

Bill Of Materials in SOLIDWORKS Drawing

Bill Of Materials

Once you would get it looking like you want, you would want to save it out as a template so you can easily get back to same style.  If you Right Mouse Click on the table you will get the option to save it.  You can then specify it as a Template and place it with your other ones.  The next time you start a BOM, you will want to choose the one you just saved out and the columns and font will be the same.
Save as template in SOLIDWORKS Drawing
When you RMC, you will notice you can save the BOM as an excel file.  Now with it in excel, you can import it to an ERP/MRP system.

Hole Table

This is used to automatically generate hole information in a tabular format.  The table will show the location and hole size from a specified origin.

Hole Table in SOLIDWORKS Drawing

Hole Table

You also have the ability to customize it with a specific font and size.  You can also add tolerances for the locations and the hole sizes.

Revision Tables

This type of table is used to represent the latest revision of the drawing.  You can see the description of the change, the date it occurred, who did it, and the revision symbol in the drawing.



The revision table can also update the Revision Block in your title block.

Weldment Cut List Tables

A cut list is similar to a BOM.  This is used with the weldment function to represent the cut lengths for structural shapes.


Weldment Cutlist

The cut list can again be customized like the BOM to show what is important for final manufacturing.  It has the same ability to be saved as a template and excel file.  This is only active when you have a part file that is a weldment.

General Table

This would be used when you need to type in data in the cells rather than having the software automatically generate the data.  You have the same ability as other tables.  You can split, merge, sort, save, etc this table just like the other types.

Weld Table

The weld table is a summary of weld specifications.  It will represent weld quantity, size, symbol, length, and other custom bead properties.


Weld Table

The table will get the data from the drawing view.  If you add the weld beads to the model, it will automatically fill the table out.  If you are only placing the weld symbols on the drawing views, there is an option in the property manager to include drawing annotations.

Bend Table


Bend Table in SOLIDWORKS Drawing

Bend tables are used with Sheet Metal parts.  In place of having many callout for each bend, you can represent these in a table.  It will specify the bend direction, the angle that it needs to bend to, and the radius of the bend.

Punch Table


Punch Table in SOLIDWORKS Drawings

Punch tables are also used with Sheet Metal parts.  This is very similar to hole tables but in place of holes, it is used with form features.  The table will represent the location of the punch on the flat pattern, the punch ID, the quantity, and the angle between the X-axis and the tool.

Thank You

This was just a high level overview of SOLIDWORKS tables.  If you have any specific questions about them, don’t hesitate to contact us.

Josh Spencer

Elite Application Engineer, CSWE 3DVision Technologies

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.


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:


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.


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

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