Resize text...

I need to resize extruded text in a part from a design table.The problem is that there doesn't seem to be a way to attach adimension to text. Can someone think of a way to do this with code?

I've attached a simple part as an example. The way it should workis that changing the height and width of the base extrusion shouldcause a change of the height of the extruded text. D2@Sketch2should drive the text height but it is totally disconnected in thiscase (just change the height of the base extrusion to verify this).

Thanks,

-Martin

SolidworksApi macros
Answers 8
SF
SF 2008-12-10 Best Answer
Just add a Link Values relation to the 2 dimensionsD1@Extrude1 and D2@Extrude2. Select both dimensions, right-click,Link Values
SF
SF 2008-12-11
You misunderstood my problem. What you are suggesting doesnot link any one dimension to the height of the text. I need toparameterize text height.

-Martin
SF
SF 2008-12-11
Ah right not the depth then I get you now.

You already have equations set up to work out the height of thetext, just alter the equations to incorporate the Extrude1's depthas a factor
SF
SF 2008-12-11
I apologize, I have obviously failed to make my problem clearenough. I'm sorry. I'll try again:

I need to be able to control text HEIGHT parametrically, preferablyfrom a design table.

When you enter text into a sketch there is no such thing as adimension ON THE SKETCH that determines the HEIGHT of that text. Inorder to modify the HEIGHT one has to use the font selection dialogand manually alter that value. As far as I can tell there is no wayto "touch" text HEIGHT from an equation.

I have a part (an injection molded emblem) that needs to bemanufactured in various sizes. I can parameterize every feature ofthis emblem with the exception of text height. I can drive partdimensions, extrusion depths, etc. from a design table just fine.No such luck for text height. I really want to avoid having tomanually edit text height every time a new size emblem is required.This is opening the door for errors.

Anyhow, I thought that, just maybe, there's a way to use the API tocreate a link between a dimension somewhere on the same sketch thatthe text is on and the height of the corresponding text. Can anyonehelp me with this?

Thanks,

-Martin
SF
SF 2008-12-12
You cannot do it with a design table but in API what you needto do is get the SketchText object and set its format, for examplethis will work on your part:

Option Explicit

Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim SelMgr As SelectionMgr
Dim text As SketchText
Dim format As TextFormat

Sub main()

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc
Set SelMgr = swModel.SelectionManager

swModel.Extension.SelectByID2 "Sketch2", "SKETCH", 0, 0, 0, False,0, Nothing, 0
swModel.EditSketch
swModel.Extension.SelectByID2 "SketchText1", "SKETCHTEXT", 0, 0, 0,False, 0, Nothing, 0
Set text = SelMgr.GetSelectedObject6(1, -1)
Set format = text.GetTextFormat
format.CharHeight = 1 ' set size you want based on dimensions here
text.SetTextFormat False, format
swModel.EditRebuild3

End Sub



YN
YN 2014-07-15

Private Sub ll1()

  Dim SwApp As SldWorks.SldWorks, SwModel As ModelDoc2

  Dim SwSelMgr As SelectionMgr, SwFeat As Feature

    Set SwApp = GetObject(, "SldWorks.Application")

    Set SwModel = SwApp.ActiveDoc

    Set SwSelMgr = SwModel.SelectionManager

    Set SwFeat = SwModel.FeatureByName("草图1")

  Dim SwSketch As Sketch

    Set SwSketch = SwFeat.GetSpecificFeature2

  Dim vSkSeg, vSkSegArr, SwSkSeg As SketchSegment

    vSkSegArr = SwSketch.GetSketchSegments

  Dim SwSkText As SketchText

    For Each vSkSeg In vSkSegArr

      Set SwSkSeg = vSkSeg

      ''

      Select Case SwSkSeg.GetType

            Case swSketchLINE

                Set swSkLine = SwSkSeg

            Case swSketchARC

                Set swSkArc = SwSkSeg

            Case swSketchELLIPSE

                Set swSkEllipse = SwSkSeg

            Case swSketchSPLINE

                Set swSkSpline = SwSkSeg

            Case swSketchTEXT

                Set SwSkText = SwSkSeg

                Debug.Print SwSkText.Text

                Debug.Print SwSkText.GetUseDocTextFormat ', SwSkText.GetTextFormat

               

            Case swSketchPARABOLA

                Set swSkParabola = SwSkSeg

            Case Default

                Debug.Assert False

        End Select

    Next

End Sub

SP
SP 2014-07-15

Check out this video of equation triggered macros. It might help you out.

http://www.cadsharp.com/blog/equation-triggered-macros/

YN
YN 2014-07-15

***************

Username: ning58,Password: 44bfc25

You may log in and start learning the SolidWorks API right now.

but don't see videos in your web site like videos.

*********************

Hope  see the following content

Lesson 1.1 – Introduction to VBA 

Lesson 1.2 – Using variables 

Lesson 1.3 – Using arrays