No dimensions on drawing

[Jacoolo]

I have a drawing of assembly where dimension disappear after View>Update>Current sheet



It happens only for dimension which are created in drawing, not those ones by Show\Erase tool(from model or assembly)



All layers are unhide. The dimensions can be found be search tool,
after selcting they highlight in red color but after updating the the
drawing they disappear.



I tried to show them by saerch tool than make save, but when the drawing is opened there are no dimension.



In addition I noticed some error in message area



View attachment 1646



another info is that "the drawing is more recent than the model"



Any ideas?

 

[caddie]

Try the config.pro option "create_drawing_dims_only" set to "Yes"

 

[Jacoolo]

This is already implemented but thanks





Any other ideas?

 

[shashiproe]

Hi,


Make sure that, is your given dimensions are assigned to other layer which is hide.


Try to unhide all layer one by one and see the effect.


If found you will catch those layer and remove the dimensions from it.


Hope this idia will work...


Regards,


Shashi
Edited by: shashiproe

 

[Isair]

Maybe your geometry of model was drastically changed so dimension lose reference, and view lose geometry that was reference for it.
You are referring to "the drawing is more recent than the model" case and I think that this is exactly that.
You didn't mention which release of Pro/E you use.

 

[mudassirkhan]

In addition I noticed some error in message area

View attachment 1698

another info is that "the drawing is more recent than the model"

Any ideas?

Hello muadib3d


The first warning occurs when u miss some reference required for view creation hence to rectify this warning just redefine ur view by using new references in place of old.


The next warning regarding partial view is because of the origin point taken during partial view creation is missing. This may be because of some fillet or edge deleted during modifications. The solution to this is same, simply redefine ur partial view with new reference.


Regarding ur last warning, this occurs when the version of ur model and drawing are different. You have to take a backup of the drawing to solve this problem.


Hope this helps,


Thanks and Regards

 

[Jacoolo]

Thanks to all


well as I wrote I checked all layers and switched them to unhide but It not works

what is strange it happens only for dimensions which are created in drawing ,not those ones which come from model(show\erase)


this happened first time

my version of Pro\e is WF 2.0 M110

 

[BONES1369]

I have had the exact same issue, (using wildfire 2) if I create a dimension in the drawing, it shows up as a reference dimension, and once I close pro-e and open again the next day, it is gone. I have found no solution other than creating a datum plane in the model as an offset to get the proper dimensions to be a show/erase dimension.

 

[Jacoolo]

thanks bones


unfortunately I can not afford for this. My drawing is for assembly and I should not add any unnecessary elements to assembly

 

[Isair]

Try with this config option:


save_modified_draw_models_only set to Yes


I have similar case to yours muadib but my problem was I working on model and coworker worked on drawing on different working directory. After we put files together and open drawing all dimensions (except that what was created with show/erase) ware gone.
That happened because model from which drawing was made have .prt.5 and model I was working on have .prt.8 (notice: when you create drawing ProE stores drawing information into part).

 

[dr_gallup]

What you need is:

create_drawing_dims_only YES

This will save created dimensions in the drawing and not in the model.

 

[arroyopr]

I agree with dr_gallup. I had this problem long time ago and that's exactly what I did, never ever had the problem again.

 

[dr_gallup]

Oops, I missed the earlier post that said that had already been tried & it did not help. Make sure this is not getting overridden somewhere in a later config.pro. Maybe put it in the config.sup.

 

[pcomeau]

We have had a similar issue I posted this morning. I will try this config option. Thanks!
Below is my post:

<h2><a href="http://communities.ptc.com/message/161487#161487" target="_blank">Dimensions
have left the building!</a></h2>
<div ="jive-rendered-content">

The issue we are having is when
using older pro version parts or backing up a multi sheet-drawing
package to use for a similar project to

 

[krow72]

You say they can be found by search tool. Have you tried to change the "smart" pulldown to dimension and try to pick them that way?