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Diameter Symbol Not Showing in Feature Sketch Dimensions

Question asked by Nick Tzallas on Jan 23, 2018
Latest reply on Feb 7, 2018 by Nick Tzallas

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I seem to be having some trouble with the Diameter Symbol not showing up in the diameter Dimensions of features.

This is not the same as the <MOD-DIA> issue

I dimension the sketch as a diameter across a centerline and yet the Diameter symbol does not appear in the dimension. Nor does it carry over into the drawing.

I though that maybe a made a mistake and the sketch dimension was recognized as linear instead of diametrical/radial but if you click on the dimension it does give you the option to switch to radial. Also the leader options in the dimensions property manager do have radial/ diametrical selections available

So I would assume that it is indeed being picked up as a diameter dimension

Is there some setting in my document properties or somewhere else that I have forgotten to select/deselect? or anything else I might have missed?

This is driving me bonkers

Using a slightly modified ANSI document property standard

SW 2016 SP 3.0

Win10 Pro 64bit

Nick Tzallas Feb 7, 2018 6:00 AM

Correct Answer

Kenneth Barrentine thank you for the trouble shooting there.

I do believe I have found the culprit after having a thought about what you did.

I have Master Axes in the part/assembly templates.

When you select the "master axis" as the revolution axis in a revolved feature, it is not recognized as a diameter, since , I guess, SW does not "see" it as in situ and therefore, does not place the Dia symbol.

If you use the Centerline created within the feature sketch then the Dia Symbol is placed correctly.

I think that's why it popped up for you when you created it since you, by default, let it use the sketch centreline as axis of revolution.

**Edit: I should mention that the diameter symbol will indeed appear but after the revolved feature is created. In sketch mode, during generation of the dimension, the dia symbol is not present. Once revolve is applied the dia symbol appears.(at least in my particular case) Just to clarify.

Hope that clears things up. Hopefully there might be a Service/enhancement request to make it recognize both?

Thank you all for the help!

See the reply in context

No one else had this question

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Josef Kasik Jan 23, 2018 1:23 AM

Hello Nick,

The first is SolidWorks application restart, turn it off and on again, you know Next, maybe try to check, if the gtol.sym file is not corrupted. In the default you can find it here - C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2016\lang\english. Try to copy another gtol.sym file from a computer with no issues. The last think what I can recommend is try to use default file templates with a default Drafting Standard.

Hope it helps.

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Nick Tzallas @ Josef Kasik on Jan 23, 2018 2:04 AM

Thank you Josef Kasik

I tried the SW restart and there is no difference I'm afraid

gtol.sym file does not seem to be corrupted. However, if someone has a confirmed uncorrupted copy of the gtol.sym file from SW 2016 and they could upload here so I could try it out, that would be a great help

That said, logically (?) it should not be a symbol library corruption issue since the <MOD-DIAM> symbol does indeed:

exist
comes up when typing <MOD-DIAM> manually in dimensions
manually clicking the symbol to add it to dimensions
appears automatically as it should in other diameter dimensions of feature sketches (e.g. extrusion boss profile below screen shot)

In the same part file, one profile feature from an extrusion does display the diameter symbol correctly, whilst in the revolved cut feature sketch it seems to not be picked up as per original post.

Below screenshot: if i add it manually symbol appears in the dimensions in question.

below section of the screenshot, shows existing automatically recognized diameter symbol placed in an extruded boss feature.

both from same part file

So I guess this would imply that it isn't a symbol library corruption (??)

Just thinking out loud.....Is there any chance this could be because the dimensions are linked to global variables ?

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Nick Tzallas Jan 30, 2018 5:11 AM

Does anyboday have any further insight on this?

It is driving me mental. Can't figure it out.

Actions

Kenneth Barrentine @ Nick Tzallas on Feb 1, 2018 4:13 PM

You mentioned restarting SW with no effect.

Have you restarted the PC?

Is it just one file or all files?

Is it just with revolves or all features?

Can you attach the problem part or a simplified version of the problem part?

Actions

Nick Tzallas @ Kenneth Barrentine on Feb 6, 2018 6:26 AM

Kenneth Barrentine thanks for the reply

To answer your questions:

Kenneth Barrentine wrote:

You mentioned restarting SW with no effect.
Have you restarted the PC?

Is it just one file or all files?
Is it just with revolves or all features?

Can you attach the problem part or a simplified version of the problem part?

Restarted PC and SW numerous times - No difference

Its any file. Global behaviour. Anything created with current setup has the same issue

It is only with revolved features. For extrusions etc, the symbol appears as normal

Have attached a sample part created from part template. "stock feature" is default in template and shows Diameter symbols as usual.

"test Revolved Cut for Dia symbol" is a revolved feature to show that it does not place the diameter symbol in those cases, despite recognizing it as a diameter/radial dimension as mentioned in OP.

I have also attached my modified ANSI drafting standards, in case the culprit is in there somewhere.

I don't now if the SW setup file would offer any insight either ?

Not sure what else could be of use to you, please let me know

Cheers

Attachments

SPL ANSI-Modified Make Part Drawing.sldstd.zip1.8 KB
SPL ANSI-Modified Model.sldstd.zip1.7 KB
Part1.SLDPRT.zip81.8 KB

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Kenneth Barrentine @ Nick Tzallas on Feb 6, 2018 10:13 AM

Well I certainly can't explain this one.

First I loaded our drafting standard, no change.

Then I saved as 2017, no change.

I tried several other things but the simplest was this.

Drafting standard is yours.

Open part1,

Deleted the revolve cut and sketch.

Created a new revolve cut and viola, diameter symbol.

Nothing else was modified.

File is still at 2016 I haven't saved yet.

Attachments

Diameter.jpg289.2 KB

Actions

Nick Tzallas @ Kenneth Barrentine on Feb 7, 2018 6:00 AM

Kenneth Barrentine thank you for the trouble shooting there.

I do believe I have found the culprit after having a thought about what you did.

I have Master Axes in the part/assembly templates.

If you use the Centerline created within the feature sketch then the Dia Symbol is placed correctly.

I think that's why it popped up for you when you created it since you, by default, let it use the sketch centreline as axis of revolution.

Hope that clears things up. Hopefully there might be a Service/enhancement request to make it recognize both?

Thank you all for the help!

Actions

Igor Fomenko @ Nick Tzallas on Feb 6, 2018 6:38 AM

It`s absolutly normal behavior of SW, it puts <MOD-DIM> prefix automatically only for circular segments.

Actions

Nick Tzallas @ Igor Fomenko on Feb 6, 2018 6:30 AM

Igor Fomenko are you positive?

I could have sworn that in older versions (e.g. SW 2014) the dia symbol was applied to revolved profiles too. I specifically created several drawings for my previous employer and never encountered this particular issue, hence why it is perplexing me so much.

Maybe this is some sort of "enhancement" ??

Hopefully Kenneth Barrentine or anyone else for that matter, might be able spot something for the both of us.

Cheers

Actions

Igor Fomenko @ Nick Tzallas on Feb 6, 2018 6:47 AM

Yes,I`m positive. There is no difference between centerline and symmetry line in SW. Sometimes centerline can be symmetry line at the same time. So I think at one moment SW decided to remove 'old' automatic behavior.

Actions

10 Replies

Josef Kasik Jan 23, 2018 1:23 AM
Mark Correct
Correct Answer
Hello Nick,
The first is SolidWorks application restart, turn it off and on again, you know Next, maybe try to check, if the gtol.sym file is not corrupted. In the default you can find it here - C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2016\lang\english. Try to copy another gtol.sym file from a computer with no issues. The last think what I can recommend is try to use default file templates with a default Drafting Standard.
Hope it helps.
Like • Show 1 Like1
Actions
- Nick Tzallas @ Josef Kasik on Jan 23, 2018 2:04 AM
  Mark Correct
  Correct Answer
  Thank you Josef Kasik
  
  I tried the SW restart and there is no difference I'm afraid
  gtol.sym file does not seem to be corrupted. However, if someone has a confirmed uncorrupted copy of the gtol.sym file from SW 2016 and they could upload here so I could try it out, that would be a great help
  
  That said, logically (?) it should not be a symbol library corruption issue since the <MOD-DIAM> symbol does indeed:
  exist
  comes up when typing <MOD-DIAM> manually in dimensions
  manually clicking the symbol to add it to dimensions
  appears automatically as it should in other diameter dimensions of feature sketches (e.g. extrusion boss profile below screen shot)
  
  In the same part file, one profile feature from an extrusion does display the diameter symbol correctly, whilst in the revolved cut feature sketch it seems to not be picked up as per original post.
  
  Below screenshot: if i add it manually symbol appears in the dimensions in question.
  below section of the screenshot, shows existing automatically recognized diameter symbol placed in an extruded boss feature.
  both from same part file
  
  So I guess this would imply that it isn't a symbol library corruption (??)
  
  Just thinking out loud.....Is there any chance this could be because the dimensions are linked to global variables ?
  Like • Show 0 Likes0
  Actions
Nick Tzallas Jan 30, 2018 5:11 AM
Mark Correct
Correct Answer
Does anyboday have any further insight on this?
It is driving me mental. Can't figure it out.
Like • Show 0 Likes0
Actions
- Kenneth Barrentine @ Nick Tzallas on Feb 1, 2018 4:13 PM
  Mark Correct
  Correct Answer
  You mentioned restarting SW with no effect.
  Have you restarted the PC?
  
  Is it just one file or all files?
  Is it just with revolves or all features?
  
  Can you attach the problem part or a simplified version of the problem part?
  Like • Show 1 Like1
  Actions
  - Nick Tzallas @ Kenneth Barrentine on Feb 6, 2018 6:26 AM
    Mark Correct
    Correct Answer
    Kenneth Barrentine thanks for the reply
    
    To answer your questions:
    
    Kenneth Barrentine wrote:
    
    You mentioned restarting SW with no effect.
    Have you restarted the PC?
    
    Is it just one file or all files?
    Is it just with revolves or all features?
    
    Can you attach the problem part or a simplified version of the problem part?
    Restarted PC and SW numerous times - No difference
    
    Its any file. Global behaviour. Anything created with current setup has the same issue
    It is only with revolved features. For extrusions etc, the symbol appears as normal
    
    Have attached a sample part created from part template. "stock feature" is default in template and shows Diameter symbols as usual.
    "test Revolved Cut for Dia symbol" is a revolved feature to show that it does not place the diameter symbol in those cases, despite recognizing it as a diameter/radial dimension as mentioned in OP.
    
    I have also attached my modified ANSI drafting standards, in case the culprit is in there somewhere.
    I don't now if the SW setup file would offer any insight either ?
    
    Not sure what else could be of use to you, please let me know
    
    Cheers
    Attachments
    SPL ANSI-Modified Make Part Drawing.sldstd.zip1.8 KB
    SPL ANSI-Modified Model.sldstd.zip1.7 KB
    Part1.SLDPRT.zip81.8 KB
    Like • Show 0 Likes0
    Actions
    - Kenneth Barrentine @ Nick Tzallas on Feb 6, 2018 10:13 AM
      Mark Correct
      Correct Answer
      Well I certainly can't explain this one.
      
      First I loaded our drafting standard, no change.
      Then I saved as 2017, no change.
      I tried several other things but the simplest was this.
      
      Drafting standard is yours.
      Open part1,
      Deleted the revolve cut and sketch.
      Created a new revolve cut and viola, diameter symbol.
      Nothing else was modified.
      
      File is still at 2016 I haven't saved yet.
      Attachments
      Diameter.jpg289.2 KB
      Like • Show 1 Like1
      Actions
      - Nick Tzallas @ Kenneth Barrentine on Feb 7, 2018 6:00 AM
        Unmark Correct
        Correct Answer
        Kenneth Barrentine thank you for the trouble shooting there.
        
        I do believe I have found the culprit after having a thought about what you did.
        
        I have Master Axes in the part/assembly templates.
        When you select the "master axis" as the revolution axis in a revolved feature, it is not recognized as a diameter, since , I guess, SW does not "see" it as in situ and therefore, does not place the Dia symbol.
        
        If you use the Centerline created within the feature sketch then the Dia Symbol is placed correctly.
        
        I think that's why it popped up for you when you created it since you, by default, let it use the sketch centreline as axis of revolution.
        
        **Edit: I should mention that the diameter symbol will indeed appear but after the revolved feature is created. In sketch mode, during generation of the dimension, the dia symbol is not present. Once revolve is applied the dia symbol appears.(at least in my particular case) Just to clarify.
        
        Hope that clears things up. Hopefully there might be a Service/enhancement request to make it recognize both?
        
        Thank you all for the help!
        Like • Show 0 Likes0
        Actions
- Igor Fomenko @ Nick Tzallas on Feb 6, 2018 6:38 AM
  Mark Correct
  Correct Answer
  It`s absolutly normal behavior of SW, it puts <MOD-DIM> prefix automatically only for circular segments.
  Like • Show 1 Like1
  Actions
  - Nick Tzallas @ Igor Fomenko on Feb 6, 2018 6:30 AM
    Mark Correct
    Correct Answer
    Igor Fomenko are you positive?
    I could have sworn that in older versions (e.g. SW 2014) the dia symbol was applied to revolved profiles too. I specifically created several drawings for my previous employer and never encountered this particular issue, hence why it is perplexing me so much.
    
    Maybe this is some sort of "enhancement" ??
    
    Hopefully Kenneth Barrentine or anyone else for that matter, might be able spot something for the both of us.
    
    Cheers
    Like • Show 0 Likes0
    Actions
    - Igor Fomenko @ Nick Tzallas on Feb 6, 2018 6:47 AM
      Mark Correct
      Correct Answer
      Yes,I`m positive. There is no difference between centerline and symmetry line in SW. Sometimes centerline can be symmetry line at the same time. So I think at one moment SW decided to remove 'old' automatic behavior.
      Like • Show 1 Like1
      Actions

Diameter Symbol Not Showing in Feature Sketch Dimensions

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