How are you using the "create_drawing_dims_only" config.pro option?

[Mfridman]

Hello all,

I would like to gather feedback from this community about how of the long existing "create_drawing_dims_only" config.pro option is being used in your organizations.

First let me provide a short summary for the values of this option

If set to NO  - when creating a driven dimension in the drawing, the dimension is stored with the model (however not visible there). this dimension can be essentially leveraged to another drawing of the same model (but is not really going with the model based approach)

If set to YES - when creating a driven dimension in the drawing, the dimension is stored with the drawing only

My impression is that many Creo users (and their CAD Admins) have set this option to be set to YES, in order to avoid pushing drawing information to the model 

Currently the default value of this option is set to a value of NO. we (PTC) are considering to change the default value of this option to be YES (which seems to be more suitable for many Creo users who are already using this value in their organizations)

So here are my questions to this community, hopefully you can help:

1. Which value are you currently using for the "create_drawing_dims_only" config.pro option, in your organization and why you prefer this value over the other?

2. Do you have any concerns from us changing the default value of this option to be YES (please note that we are not removing this option, we are just considering to change its default value to match to what seems to be used by many.

Also a change of this option will not impact any existing dimensions in your drawings, it applies ONLY to newly created dimensions

I would appreciate any feedback on the above

Thanks and regards

Michael Fridman

Creo Product Manager

[pausob]

This is a very good idea.  AFAIK, this default option (create_drawing_dims_only=no) is so useless except for generating confusion from users about why their dimensions disappeared after checking in the drawing (but not the model) or if the model they were detailing was changed by the designer and they updated to latest in their workspace or some nonsense like that.

And you are keeping it around, which is good because options are always good.  While you are tackling this - consider making a tool available in the annotate tab which would take the driven dimensions generated in the drawing (and stored in the model with that option set to no) - and make them be "shown" in a model's combined state (often, it's just way easier to dimension on 2D drawing vs. on the 3D model)...

[Mfridman]

Hi @pausob 

So, based on your answers, I assume that you are using the YES value for this option.

I would agree that the value NO, might be confusing in some situations, it is a legacy behavior and the config was added later in order to resolve some of the confusion.  

Thanks for the feedback 

[Chris3]

We have it set to yes. It was set before my time and honestly I have never bothered to consider why. I have no concerns changing the default.

[StephenW]

Creo 4, NO MBD and NO plans to go to MBD.

We have it specifically set to NO in our config.pro to allow GD&T created in the model to be attached to the created drawing dimensions. As far as I know, this was the only reason we have it set to NO.

We do not have strict controls on model changes so allowing the model to be changed during the drawing process is acceptable and expected by most users, especially when the drawing is intentionally being changed.

Since we are still on Creo 4, a shift in PTC's default in a future release wouldn't affect us in the near term. 

[Mfridman]

Thanks for the feedback @StephenW  

I do have a follow up question for you:

The only thing that is not clear to me is why would you prefer to change attachment of model gtols that are shown in the drawing and place them on dimensions that are created from the drawing? 

Wouldn't it be more robust for you, if you create both of them (dimension and the gtol) on the same object (model or drawing)? 

Ideally, I would say that creating both the gtol and the dimension that the gtol is placed on, directly on the model side and then shown in the drawing would be the preferred way. that would make sure that whatever changes you are doing to it in the model are propagated to all of the drawings of the same model and there is no mix of workflows.

If you do not like the model based way since MBD is not on your roadmap, you can always create the gtol and the dimension both in the drawing itself, and have them be drawing owned only. this will eliminate the mix of model owned & drawing owned 

[StephenW]

Soooo, based on my experience from Pro/E, it was always easier to create datums in the model and then GD&T while in the drawing but "in the model" as that was an option available in the past. But, a lot of the time, I would be doing GD&T on models that didn't necessarily have the correct model dimensions to show (likely due to poor practice) so the dimensions were created in the drawing and the GD&T was "attached" to the created dimensions, hence the need to create drawing dims in model.

I will also say that at some point a few years ago, someone had added the create drawing dimensions YES option in our standard config.pro and I was the one who complained after someone asked me why they couldn't do their GD&T like they used to. 

I think ideally you are correct that having all the "stuff" in either the model or the drawing would be wise.

I haven't done much GD&T lately. I know the entire workflow has changed a lot AND I am currently using creo 4 so you know  better than me what has changed since then. Most of my notions of how GD&T is done in Creo is based on my Pro/E wildfire and before experience and NOT based on any current software capabilities.

[TomU]

It is set to YES in our config.sup so no one can change it.  It's been that way for at least 15 years.

[kdirth]

It is set to "no" here.  Being the default setting, that is what we have as it has not been defined in our config files.  I am sure it has never been looked at here.  I believe this is the correct setting for us as we have one drawing for each model.  Also, if this affects attaching GD&T on our drawings, as @StephenW indicated, we would want to keep it at no.  I don't see us going to MBD anytime soon. 

If you do change it, make sure it is communicated in the release so everyone using no will know what to expect and what to change to get back to "normal"

[Mfridman]

Hi @kdirth , thank you for your feedback

Since you said that you are creating one drawing for one model, what is the benefit for you to be storing the dimension that was created in the drawing, with the model? 

For GD&T, you can add all of your annotations directly in the model and simply show them in the drawing (more closely related to model based approach and would cause less sync problems between 3D/2D objects)

OR 

you can also use this config option with a value of YES - this will cause creation of dimensions in the drawing to be stored only with the drawing itself (drawing owned). in parallel, you can create drawing owned gtols which will be placed on those dimensions, if needed (Drawing owned annotation approach)

I personally find the first option preferred, as this would make your design to be more robust in case that you will have additional drawings created for the same model in the future (as well as it would take you one step closer to MBD, when the day comes for your organization to consider it. and also less legacy data to convert to the model based way) 

[kdirth]

Until today, I did not know the config option existed.  It has always been at default for me.  I can see some benefit to setting it to yes to prepare for the possibility of switching to MBD in the future.  I think the biggest change for us would be in creating GD&T, which we use sparingly. 

I have never had the need for more than one drawing for a part or assembly.  Nor do I think it would be a good idea.  The only place I could see that is with family tables.  And, outside of hardware, most seem to avoid family tables like the plague.

[RandyJones]

We have it set to yes in our system config.pro. Has been that way since the late 90's.

[Mfridman]

Great, thanks for the feedback

[mkajdan]

We have this config set to YES also.  Our config.pro history only goes back to 2010 so it has been set to YES at least that long, probably longer.

[Patriot_1776]

I've had it set to yes since I was on V15 in the mid-'90's.  I don't want all the things I do in my drawing cluttering up my model, or worse, forcing Windchill to modify the model (change iteration) and force me to check it out.  As an "Olde School" guy who started off on the drafting board in the early '80's, I don't LIKE the MDB ONLY mentality.  In my professional opinion, there will ALWAYS be a place for drawings.  The welder doing a field installation is NOT going to have a fragile i-pad or similar while he's working the job.  The machinist does not have a CAD station handy (even if he knew how to use it) and WANTS to have a drawing handy.  Plus, you can easily write on your copy of the dwg, make notes, do mark-ups, etc.  Now, with later versions of ASME Y14.5, you can use the "all-over" for profile tolerance which is what I use for all but critical dimensions, and thread callouts and such.  I'll show overall dimensions in basic, those that I want controlled by a profile (or other) tol that's tighter than the "all-over" tol, and that's it.  It makes the drawings a LOT easier since I don't have to dimension every single feature, I just have a note 1 that says it's a "reduced-dimension model-based drawing" and to follow the "all-over" profile tol for everything not specifically dimensioned.  Since we switched to Creo 4, I no longer even crate ASME datums at the model level, I only create drawing datums.  Makes things MUCH simpler, and besides, I was getting REALLY annoyed at the errors telling me I had legacy datums.

So, long story short, I think it's a good idea to make the default setting "yes", since it seems the vast majority of us set it that way anyway.

Here's a better idea:  Get rid of the "hidden" config settings and make them visible.  We're adults here (well, me excepted), and can make our own decisions on settings.

[rzukowski]

In my company, we have the option "create_drawing_dims_only" set to YES.  It's been this way for as long as I can remember (20+ years ?).  Our intention is to have the model drive the drawing, not the drawing drive the model.  There some instances where the design intent of the modeling is different than the way the part is manufactured.  An example is with water lines in mold inserts:

• We design the water lines relative to the molding surfaces so that the offset distance stays constant regardless of the insert size, ie: from the parting-line down.
• However, we detail the water lines relative to the back of the insert block, because in most cases with core half inserts, the parting-line elevation does not exist until later in the manufacturing process: drill first, rough second.

[BG_9869104]

I want everything saved in the model and shown on the drawing. So I have create_drawing_dims_only NO.
I have found that there is a bug(7.0.3 and other versions) of gtols datum labels saved to the model can become lost datum labels and cause datum already used warnings even if it is not used.

I am not providing 3D MBD models with combine states and dimensions shown in 3D to suppliers/users. I am trying to move to storing all model definition in the models. 2D drawings used to shown model dimensions, model parameters, and model notes. So this in a hybrid case of yes the model has all the definition but no dimensioning drafting is done in 3D. All the Drafting/detailing is done in 2D through show dimension, model notes, model parameters.

[Mfridman]

Thanks a lot for the feedback @BG_9869104 , however I am little confused by your answer. maybe you can help to clarify this for me

you say that you are doing all the model definition in the model and the drawing is used to show dimensions etc.

So those shown dimensions are actually model dimensions.

If you are anyway mostly showing the model dimensions in the drawing (meaning that they are model dimensions that are simply shown in the drawing), so why would you want this config to be set to a value of NO then?

[BG_9869104]

Yes saves to drawing.

No saves to solid model. 

I want to save to model so No is the option for me.

Sometimes edits/fix can be done in DRW mode. I want what can be saved to the model to be saved to the model.

[TomU]

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@BG_9869104 wrote:

Yes saves to drawing.

No saves to solid model. 

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I don't think that's accurate.  Even with the option set to 'yes', changes made to shown dimensions are still saved back to the model.  The big difference is where created dimensions are saved.  With it set to 'yes', dimensions created in the drawing are saved to the drawing.  With it set to 'no', dimensions created in the drawing are saved to the model.  This does not apply to shown dimensions (unless I'm wrong.)

[BG_9869104]

Both are correct. Since legacy models are also dealt with and getting multi users to do it the corporate way is always a struggle there are cases of adding annotations in DRW mode. 

From the help

yes - Save all new dimensions created in the drawing inside the drawing as associative draft dimensions.

no* - Save all dimensions created in drawing mode in the part.

It is a slow transition to get all model information saved into the models. Legacy parts in production that will not be messed with for backend changes are a big hold up. That and time.

The biggest difference I see with this setting is the need to have the model available for edit the same time as the DRW when set to NO. If set to Yes then the DRW can have annotations added without the model being checked out. 

[Mfridman]

@BG_9869104  Model checkout is indeed required when this setting is set to NO. Not everyone accepts this as desired behavior either, but it is tied to the way that your organization works.

So to summarize, while you prefer to use the value NO for this option, do you have any concerns if the default value for this option will be changed to YES ? 

If that change will be applied, we will off-course make sure that we communicate it clearly in the release/what's notes, so that those who uses the value NO will be able to update the default if required 

[Mfridman]

This is correct. the config option talks about dimensions that are Created in the drawing and being saved with the drawing/model (according to the chosen setting)

[MichaelToledano]

Hi Michael,

We use this 'create_drawing_dims_only' config.pro option with the value of 'YES'.

As each model is drawn in a single drawing (in the vast majority of cases), we do not have the need to utilize driven dimensions elsewhere outside the scope of that single drawing.

Best Regards, 

Michael

[Mfridman]

Thanks a lot for your feedback Michael