Is it possible to set default decimal places on creo drawing?

[pimm]

I am using Creo version 7.

My system decimal places are 5.

My drawing decimal places need to be 3.  

Is there a way to set the default drawing decimal places to 3?

Presently I need to place all of my dimensions and then when they are placed I need to select each dimension to change them from 5 to 3 decimal places.  I keep thinking that there should be a way to modify the default drawing decimal places whether it be on the drawing template or in the config options but I just never found this.  Just to be clear I need the system decimal places to be 5 as there is a large positional difference on curvature within a given sketch unless the decimal places are increased to preserve the needed position.

[tbraxton]

Set the value of the default_dec_places configuration option for linear dimension and default_ang_dec_places for angular dimensions to required number of decimal places. Any dimension that you create will appear with the defined decimal places.

[BenLoosli]

These options are set in your drawing DTL file, not config.pro.

You will need to update any drawing templates as the DTL settings are copied into the templates when opened.

[pimm]

Ben: This does sound promising.  I will look for how this would be set up to allow changes and how to make these changes but if you or anyone knows how this could be done it would be very helpful.

[pimm]

Tbraxton:  Wouldn't that alter the default system decimal places?  I need to keep the drawing decimal places independent of the system decimal places.  Changing this would change the decimal places within a sketch.

I have a feeling that what I am looking to do is not possible but I am just hoping that it can be done.

Below is the drawing setting location where it would seem that you should be able to enter whatever drawing defaults that you want, but it doesn't work that way.

[tbraxton]

@BenLoosli  is correct, the config options set decimal places in the model. If you are using annotations from the model vs creating dimensions in the drawing you may need to alter the approach to get exactly what you need.

This should clarify things for both model and drawing decimal place control.

Article - CS160736 - [Knowledge hub] How to set default or active number of decimal places to new or active dimensions in solid model or drawing in Creo Parametric (ptc.com)

[pimm]

Tbraxton:  Scrolling through the different ways to implementing varying decimal places towards the bottom of the knowledge hub document appears to refer to making a permanent change to these settings.   It also "seems" to suggest that these changes would be set up from the drawing options "lead_trail_zeroes" setting.  See attached area of this documentation.

When I click to change this however (lead_trail_zeroes) from the defaults the drop down choices don't appear to refer to making the system/drawing settings independent from each other. 

I am crossing my fingers that this change can be made but from the given choices I'm not seeing where this might be incorporated.

[pimm]

I do believe that I read the last section of the Knowledge Base documentation incorrectly, but it still appears that it is not possible to have system default decimal places separate from drawing "default" decimal places.  I have seen numerous inquiries about this but no instances of where this was accomplished.  Eventually the person looking for the answer gave up or the thread was marked locked.

Where I looked at the last segment of the documentation incorrectly was where I thought the lead_trail_zeros setting applied to the settings below that diagram.  The other settings were just separate independent settings which really only applied to how Creo handles zeros.  This wouldn't apply to what I am looking to do.

[tbraxton]

I think that the intent of leading/trailing zeroes is to control the display of significant figures in a drawing. However, some drafting standards (ASME, ANSI, ISO) have rules about this and they are not common among the standards so if you reference a standard make sure you are not violating it with a default setting.

If you need a quick fix to address this while you research config settings, you should be able to bulk select dimensions on a drawing and set the # of decimal places displayed with one UI interaction with dimension properties.

I have never specifically done exactly what you are trying to do with environment settings in model/drawing. I will admit that the interaction of detail options and config options are convoluted in some cases and are not documented well.

[pimm]

Tbraxton:  Yes, the best option in as much as what I have seen for obtaining the needed drawing decimal places has been to region select all of the placed dimensions and make the change.  Applying the same change from drawing after drawing does become cumbersome for what seems to be a simple to implement drawing option.

I appreciate that you have verified this for me.  I haven't submitted a feature request in a number of years but perhaps this might be one to ask for. 

[tbraxton]

FYI

The config and dwg detail options discussed here control the display of significant figures and do not alter the precision of numbers used by the geometry kernel of Creo to calculate the geometry of a model.

[pausob]

I have couple of more cents to add to this thread.

Note these two config.pro options will affect how newly made or shown dimensions behave:

round_displayed_dim_values
default_dim_num_digits_changes

[pimm]

This does sound interesting but it's a little unclear whether this implementation would help or add some kind of issues.  It might be a good idea to try this out and see whether it does accomplish that which is needed.

[BenLoosli]

After experimenting and dep looking, I do not find a DTL file setting for drawing decimal places on dimensions. It takes the default from the modeling decimal places.

Options are to create the dimensions with the modeling decimal places and then change the formatting to 3 decimal places or set the modeling decimal places to 3 places and then change them in your modeling mode to 5. When a drawing is created, the dimensions come in with 3 decimal places. Maybe a mapkey to change from 3 to 5 to make it easier,

It does seem that this should be a standard DTL file setting independent of the modeling decimal places.

[MartinHanak]

Hi,

I tried something...

I created simple model (a block) and its drawing. The drawing contains one view, shown dimensions (driving) and created dimensions (driven).

If I change decimal places of shown dimension then Creo changes dimension color and after regeneration model geometry is modified.

If I change decimal places of created dimension then everything works as you need.

[tbraxton]

As posted above: "If you are using annotations from the model vs creating dimensions in the drawing you may need to alter the approach to get exactly what you need."

Creo makes a distinction between dimensions created in the model, annotations, and dimensions created in a drawing.

@MartinHanak has done some testing for you and it would appear found a solution.

[pimm]

Hi Martin,

Could you please describe what you have tried in a little different way? 

It appears that what you are saying is to initially go with the creo setting default_dec_places with a value of 3 instead of 5 as that would be the created dimension.  If so I'm not clear as to the method that was used to convert the system decimal places back to 5 instead of 3 and have the end result of having the drawing dimensions show up with 3 decimal places.

[MartinHanak]

---

@pimm wrote:

Hi Martin,

Could you please describe what you have tried in a little different way? 

It appears that what you are saying is to initially go with the creo setting default_dec_places with a value of 3 instead of 5 as that would be the created dimension.  If so I'm not clear as to the method that was used to convert the system decimal places back to 5 instead of 3 and have the end result of having the drawing dimensions show up with 3 decimal places.

---

Hi,

please replay uploaded video.

[pimm]

Martin,

Thank you, your video adds a lot of clarity to what you were saying.

By changing the tolerance in this manner is a little simpler than what I was doing, but still this action would need done every time a new drawing was needed.

I am still seeing that it would be very beneficial for Creo to have a default drawing setting that would be similar to the config model setting default_dec_places.  Wishful thinking maybe something like default_dwg_dec_places.

[MartinHanak]

---

@pimm wrote:

Martin,

Thank you, your video adds a lot of clarity to what you were saying.

By changing the tolerance in this manner is a little simpler than what I was doing, but still this action would need done every time a new drawing was needed.

I am still seeing that it would be very beneficial for Creo to have a default drawing setting that would be similar to the config model setting default_dec_places.  Wishful thinking maybe something like default_dwg_dec_places.

---

Hi,

perhaps you could also discuss your "situation" with PTC support.

[Srinivasan_Iyer]

I am on Creo 9.x.x.x

While rummaging through the help files I came across this page. Hope this helps. I must admit that I have not tried it since the number of decimal places are set to 3 in my case.

https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/detail/About_Setting_Decimal_Places_for_Dim_Tol_Values.html#