Making Title Blocks for a company ...

[design-engine]

Using Creo 2.0

Im making a title block for a customer and am having a bit of a struggle. I'm struggling with the real estate I have for description for title block. I have &description for the Title of my drawing. Do I need to have &description2 for the words to wrap if there is not enough room for the parameter to fill out that real estate?

Question 1 How is it typically done for titles i.e. BATH TOY, LOWER HOUSING if I want lower housing to be on line 2 then I need an &description2 for the second line?

Question 2 How do I get the date&time in there to auto populate?

Question 3 I have the Creo FILE NAME called out on the Title Block using this parameter {0:&model_name}.PRT and it works great .... until I get to a Creo Assembly. Didn't think of that

STOCK UNSEEN PARAMETERS
&scale < varies with respect to the model and scale in the drawing 2:1 usually
&drawing_name <varies with respect to the Part name

DEFAULT PARAMETERS WITH STOCK CREO
&description <varies with respect to the Part name
&modeled_by <AARON R

ADDED PARAMETERS FOR NIGHT VISION TITLEBLOCK
&checked_by
&engineered_by
&mfg_by
&material
&rev <P1
&classification < MOLDED PART or MACHINED PLASTIC or MACHINED PART

 

[silverado8405]

1) yes a &description and &description2 would be the best way to put a return into the table having each one in a separate cell above/below each other.

2) &todays_date is the syntax for the date, it will populate automatically when the drawing is created, I've not used the time one so I'm no help there.

3) If what you're doing is working great for 90% of your drawings, manually change it for the other 10% that are assemblies. It may be as simple as editing that cell and changing .PRT to .ASM

If you are doing multiple pages with different models as a drawing package, add in all the models you want before you start drawing. When you make a new page it's going to fill in the title block with the information from the current part, switch to the part you want it to be then under the layout tab click sheet setup, then the down arrow in the format box and reselect the current format. That part is critical and a creo nuance. It will ask you about keeping or removing existing format tables, you can usually click remove all, and it will blow away the format and re-insert it while populating the title block with the new model's information. Handy little trick for when you forget to change models before a new page or it doesn't work like it's suppose to.

 

[krow72]

1. For the "wrap", once you finish the format, you should be able to RMB on the table cell and check the "wrap text" button then save your format. This may not get exactly what you want as it will fill the length of the cell box with text then put the rest of the text on the bottom line. (ex. it may give you BATH TOY, LOWER on the top line and HOUSING on the bottom line depending on how wide your cell is.)

3. If you take out the .prt and just use &model_name, it will work with parts and assemblies.

Here is a link with all the drawing parameters for pro-e:
http://www.cad-resources.com/System_Parameters_for_Drawings.pdf

 

[srieger]

I tried the wrap function not long after it was available and it's not very reliable. Particularly for modifications that require changes in where it wraps. I think using 2 descriptions work much better.

 

[design-engine]

thanks for your input guys.

 

[design-engine]

One more question....

I set up the parameters into the model to display correctly in the title block format. What is to stop folks who don't know that they can change the drawing by modifying the parameter instead of double clicking in the title block on the drawing table?

 

[krow72]

If they double click inside the title block and change the parameter, it will also change in the part as well. Double clicking on a parameter will bring up a parameter window. If they highlight the cell and choose properties, then it will pull up the "note properties" window and show the parameter syntax "&model_name", etc...

 

[design-engine]

Ha... I didn't know that. Thanks...

For most companies that took specific training in drawing mode, they learn the parameters drive the detail drawing. Its those engineers or non draftsman types that don't have a start part with proper parameters set up already. How do we educate those folks? Or keep them from just filling out the title block and not realizing the parameter drives the detail drawing's titleblock?

 

[dr_gallup]

IF the part has parameters the corresponding areas of the drawing format fill in automatically. If not, Pro/E prompts for input into the drawing table cells. There is no way to exit or avoid this step. At this point, the cells are converted to non-associative text with no link to the model.

To correct it at this point, you have to go into the model and add the parameters. There is a lot of room for error at this point which is why it is so important to use model templates that already have this data. A lot of companies have a mapkey or other method to automatically add the parameters as frequently there are a lot of them, they have to be spelled exactly right and they need to be the right type of parameter (integer, text, numeric, etc.). Then you need to reload the format and delete the old format tables so that they get updated properly.