Dimension missing when importing in Drw. drawing.

[Carol_88]

Hi,

I faced an issue when import drawing to a drw file. The matter as below:

I have an Ori.drw and I want to create 2 sheets with the same 2D drawing in this file.

Thus, I plotted one, then save as a new-name.drw (but common 3D data).

Next, I import this new-name.drw to my Ori.drw.

Sometimes all data completely import, both sheets remain same.

However, sometimes the plotted dimension all gone for one of the sheet, only left sketches and part drawing.

Does anyone have any idea why this happen and what should I do so that both drawing's data (dimension & sketches) are kept during import action, 

Thanks.

[StephenW]

Same 3D data, yes? Did you show dimensions or create dimensions?

When you show a dimension on a drawing for a model, you can only show that dimension one time on the drawing.

Thats my guess

[Carol_88]

Yes, both using the same 3D data. Dimensions are created.

Did you mean that if I use show dimensions, even if I create 2 sheets and manually plot it, I can still only show the dimension once?

[BenLoosli]

A shown dimension can only be shown once in any drawing. Number of sheets and plotting have no bearing on it.

To show the same dimension in a second view or sheet a second time, you have to use a drawn dimension. This second dimension should be a reference dimension per ASMY Y14.5.

[StephenW]

I did my own testing on this. I created a simple part and 2 drawings for the same part. (i did not use SAVE AS on the first drawing)

I used "import drawing/data" on one of the drawings to add the other drawing with same 3d model.

The shown dimension from the model on the imported page disappeared as expected.

The created dimensions remained (these dimensions were created twice, once in each drawing, before importing)

Next, I used the first drawing i did and used "save as' to make the second drawing.

I used "import drawing/data" on one of the drawings to add the other drawing with same 3d model.

All dimensions were missing, shown and created.

OF NOTE, I have the config.pro option create_drawing_dims_only NO. Which means created dimensions on a drawing are "stored" in the model.

When I changed the config option to YES (and recreated the dimensions in the 2nd drawing), the created dimensions remained.

So, with created dimensions, it is likely you can achieve what you want if you modify the config option.

Just a warning, this is not the only thing that this config option affects. You should do your own testing and verify that it isn't going to cause you other problems making this change. The only thing I specifically remember is that GD&T created in the model can not be attached to created dimension that are drawing only, or something like that. Its been a while since I did this testing and it could be significantly changed based on what release of Creo you are using.

[Carol_88]

Thank you for information and confirmation.

My case is created dimension disappeared.

I found that for the drawing that created dimension will disappeared when imported are those drawing that the 3D data is being modified from some old model and then both 2D & 3D data is renamed to become a new drawing.

These old and rename data are all stored in Windchill.

I am not sure whether Windchill restrict duplicate information or because the 2D drawing is not newly created and thus will disappeared upon importing. 

[StephenW]

Windchill does not do anything other than store the data. 

Did you test modifying the config.pro option create_drawing_dims_only ?

What setting are you currently using?

[Carol_88]

My config.pro option create_drawing_dims_only YES.

There is no issue when a drw. is freshly created and imported.

This created dimension disappear issue only happen when the drawing creator does not create his/her own drawing, but took an old model, modified the 3D data, then allow the 2D data to update accordingly to the 3D, then saved both 2D and 3D data as new drawing. 

I am not sure whether the above action will cause the issue to happen. 

I tried below action:

1. Edit the existing dimension (repick point on the model)

2. Create a new dimension but same point as previous, then erased the old one.

3. Create new sheet and create all the dimension again.

After import drawing:

No. 1 dimension disappeared.

No. 2 and No. 3 dimension remain.

[StephenW · Accepted solution]

No matter how old or new, if the dimension was created when config.pro option was set to NO, the dimension is stored in the model and will only show once.

The dimension is not affected by changing the option afterwards. In older versions of Creo-Pro/E, that option, by default was set to NO.

I do not believe there is a work-around for dimensions that were created when the option was NO other than recreating the dimension.

For verification, you could open a case with PTC Tech support and ask.

There is also a discussion about how PTC decided to change the default setting for this option and some explanation of the reasons for the options here:

https://community.ptc.com/t5/3D-Part-Assembly-Design/How-are-you-using-the-quot-create-drawing-dims-only-quot-config/m-p/759322

[Carol_88]

Thank you for clearing that up.