There are several issues at play here.
First, as soon as you save a model while connected to Intralink the Intralink specific parameters will become available in the model. To prove this, create a new empty part. Go and look at the model parameters. There shouldn't be any. Exit the parameter dialog and save the model. Now go back into the parameter dialog and you will see all the Intralink parameters have been created. Their creation happens as soon as the model is saved to the workspace, not after it's been checked in.
Second, the drawing itself will not contain any parameters (until it is saved) if it is created from "empty" or "empty with format". Parameters that exist in the format are not created in the drawing. If you build a drawing template, and then use it to create the new drawing from, it will contain any parameters that existed in the template. (Basically Pro/e is doing a save-as from the drawing template so any parameters that existed in the drawing template will likewise exist in the new drawing.)
Third, for notes, tables, and symbols, a drawing will search for valid parameter in the currently active model first followed by the drawing. If it can't find the parameter in either place it will then prompt your to enter a value and will replace the ¶meter string with the value you entered. If the parameter is using the ¶meter:d syntax, then Pro/e will only look in the drawing for that piece of information, it will not look at the model. If it cannot find that parameter in the drawing then it will again prompt you to enter a value and use this value in place of the ¶meter:d text.
You don't specifically say so, but I think you are trying to display the Intralink parameters for the drawing using the ¶meter:d syntax. If this is the case, then those drawing parameters MUST exist at the time of drawing creation or they will not update correctly (you will be prompted for a value). The easiest way to handle this is to create a drawing template and then use that to create all new drawings from (save it, check it in, and put it in your template folder). Now when any new drawing is created from this template it will already contain the necessary parameters for your notes/tables to read.
There is one other way you can get Pro/e to look for a specific parameter, not fail when it's not there, and not prompt you for it, but it only works for MODEL parameters, not drawing parameters. Here are the steps:
1. Create a table (or use an existing one)
2. Create a repeat region (single cell is fine)
3. Set the repeat region parameter (report parameter) to &mdl.param.value
4. Add a filter to the repeat region equal to the single parameter you want to read &mdl.param.name == <parameter name=">
5. Update the table.
Now this single cell repeat region will only display the value of the filtered parameter, and it won't fail if the parameter does not exist in the model. If for some reason you did remove the model from the drawing, you will have to update the repeat region to point to the correct new model.
Tom U.
