Drawing Issues - Missing Dimensions

[AGaribay]

Drawing Issues - Missing Dimensions
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Wildfire m190

I work for a company that produces shocks for motor sports. We have a line of about 10 types of Rear Shocks. All shocks use the same hardware at the final level. The hardware consists of 20 different iterations. We take advantage of Family Tables to incorporate this. We are having difficulties with dropped dimensions in our drawings (dimensions missing or turning blue). I am getting tired of re-producing drawings every time I open them. I

 

[appinmi]

I do not know of any limitations to "family tables". The biggest one that I did had 34 instances that controlled over 1500 features. About the dimensions that are turning "blue", are they "created diensions" while in drawing mode?, or are they driven dimensions form the family table?

 

[appinmi]

There is a config.pro option, read_famtab_file_on_retrieve, which we have set to no. We were having problems when someone toleranced an "instance" model, and it would effect all of the instances within the family table. I don't know if will help, but you might give it a try.

 

[AGaribay]

Appinmi,
I am adding dimensions as opposed to showing them due to added text on the original part drawing dimension which would not apply to the Final Assembly Drawing...if that makes sense?<?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" />

In other words, when I show the dimension in the final assembly drawing, it shows an asterisk which signifies an inspection dimension in the piece part drawing (not my idea as I know ProE has its own symbol for that). We don't want to show the asterisk.

Thanks!

 

[megaladon]

i have had family tables with 1 being 15 instances 1200+ features 10 variances also 180 instances 100+ features 120 variances so file size wont affect you


are these created dims?


if so try creating dims in the model itself


simplified reps?


1 work around maybe to add points to your model and create dims from there if you had too


also found this on the web


There have been some reports of dimensions mystically missing from drawings. The following is an explanation of what is happening to those dimensions as well as an explanation of Pro/E functionality. A dimension (e.g. ad1) created in drawing mode creates a new dimension which is stored with the part model. If the drawing is copied to a new name using the Save As function it is still going to reference the part dimension ad1. Hence if that dimension is Deleted in any drawing from that family, it will be deleted from the part and thus all drawings that use that dimension. Erasing the dimension in Drawing mode will only erase the display of the dimension in the current drawing and will not affect the part model or any other drawings that show that dimension. This should be done using the show erase menu in drawing mode. This functionality is controlled by the config.pro option CREATE_DRAWING_DIMS_ONLY. Dimensions with a dd# or add# symbol can not be used with part or assembly geometric tolerances. Thus the default for "CREATE_DRAWING_DIMS_ONLY " is set to NO so that if I have a family table of parts and I add a GD&T to one it is automatically added to all the drawing.
Edited by: megaladon

 

[tdegroot]

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[AGaribay]

Thanks for the replies. I will give some of what was suggested a try.

I believe the call is still open in regards to PTC.

I decided in the mean time to use Datum Curves and Points to help with dimension stability.

 

[Isair]

Cam721
I think that your problem is in that what have megaladon pointed; when you create dimension in drawing, this dimension references on model entities and it is put in mode (in your case instance), and if this instance isn't save, or shape of instance changed dimension disappear.
So try set this option megaladon pointed; CREATE_DRAWING_DIMS_ONLY and then see if dimension disappear.


Also you could try to create Accelerator files for family table, this way you would speed up retrieval of family table instances, and their geometry would be written in file, so when opening drawing dimensions should be on their places.


To create accelerator files; File > Instance Operations > Accelerator Options > Update


Note: be careful thou, because while creating this files, your disk space would drastically become full.

 

[AGaribay]

Very good. I will set my option to "create_drawing_dims_only.


Thanks you all for your help.

 

[AGaribay]

This totally makes sense now as we tend to re-use OR Saveas existing drawings since they are so similar.

 

[petesprada]

Hi all,


I've only just come across this problem on a colleague's project. He'd created dimensioned drawings of a part, but this part was modified by someone else in a separate directory. When the new modified part was dropped in the dimensions disappeared on the drawing. VERY frustrating!


What I don't understand is why the default config option forCREATE_DRAWING_DIMS_ONLY is NO. I am now considering changing this on our company config.pro to YES, but don't quite understand the down-side. Can someone explain?

 

[dr_gallup]

We use have used CREATE_DRAWING_DIMS_ONLY YES as long as we have been using Pro/Detail. I see no problems.