Model parameter input to populate the drawing formats

[JHoracek]

We've recently (4 weeks) switched from SolidWorks to Pro/E Wildfire and have start parts set up for our models and assemblies with parameters for "drawn by", "part no.", "material" and so on. Our 2d drawing formats have been set up to populate the appropriate fields based on the information the user inputs from the solid .prt or .asm file. Right now, using our default template, the user needs to select "tools", "parameters" and enter these fields. Like most places, there are some designers that are a little lazier than others and tend not to enter this data on their own. It's a little frustrating when you use their part in an assembly and you get no information in your BOM. Is there a setting in config.pro or some other configuration file that can be set so that when someone creates a new part using our companie's standard start part they are prompted to enter the parameters?
Thanks,
Jeff

 

[looslib]

I haven't played with our format files in a while.

When I create the drawing and use my company format, it prompts me for the values for the fields in the format.

I just created a new part in Wildfire and added the existing 2001 format and I got the prompts.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[JHoracek]

Thanks Looslib,

Our formats prompt the user as well. I would like to know if there is a way to get these prompts when a user starts a .prt or a .asm
I may use someone's .prt in my assembly before they created the 2d drawing which is where I think you're saying you do it.

Jeff

 

[ttx]

Hi,
I know that in release 2001, you can check a box called "designate" in the model parameter set up dialogue box. What this does, is display the chosen parameter or parameters when starting a new part or assembly. Maybe this is the same in Wildfire?

By the way, how do you like working with Pro/E?.....You almost never hear of anyone switching from SW to Pro/E - it's usually the other way around.

cheers,

JW

 

[JHoracek]

ttx,
Thanks for the tip but alas, the designate box is checked. There must be a setting hiding somewhere else. I'm going to put a call into PTC and update this thread when/if I get a satisfactory answer.
As far as working with Pro/E, I like it . We switched from 2-d autocad about 5 yrs ago to SW and have been working with SW since then. Through acquisitions we've become a fairly large company with facilities in other states, Canada and Europe. We were using SW, another facility was using Inventor, another Mechanical DeskFlop another 2-d ACAD. We've been trying to standardize on one platform for the last 3-4 yrs but it was not a large enough priority for upper mgmt. to want to put up the money to invest in software and training 100+ seats. We had demos done at each facility with Wildfire, SW, Inventor and CATIA. Already knowing what SW and Inventor were capable of, none of these demos made me sit back and say "wow". Pro/E and CATIA both made me say "wow". CATIA was just too expensive and for what we needed, would be like driving a ferrari to the corner store for bread. Pro/E on the other hand has so many capabilites it was almost mind boggling. Granted, we've got quite a way to go before we can properly and efficiently utilize some of these features. Overall, there are in some cases more mouse clicks to get you through some of the features in Pro than in SW or Inv. but so far, I'm happy with the companies choice to go with Pro/E. We've got some people here and I'm sure other facilites have the same situation, that have gotten so comfortable with the way they "used" to do things that are having a more difficult time making the transition while others are really embracing the opportunity. All of us, company-wide, have gone through the 1 week basic training just this month so we're all "newbies" and sometime struggle with basic functions but I think that would be the case regardless of platform.
So far though I think it's great.

Jeff

 

[ttx]

Jeff,
Thanks for your comments.
I have never doubted the power of Pro/E. As I have often heard said, "There is almost nothing that Pro/E can't handle - figuring out how to do it is another matter........"
Being the CAD Administrator and a full-time Mechanical Designer, I have often wondered whether there would be less Admin. stuff to do with Solid Works. We have spent many, many hours customizing Pro/E so that it would work well with our company structure. Seeing as we are a small company, I would have rather put those hours into other things.

Thanks again and enjoy the power of Pro

JW

 

[JHoracek]

JW,

I'm pretty much in the same shoes as you, mechanical designer/appointed CAD administrator. I too would rather focus on the design work. There is much less administrative stuff with SW. Since we're all new at this Pro/E stuff here at this company, I hope the administrative stuff will calm down after a while (please don't dash my hopes by telling me it won't). Anyway, I got an answer to my question from PTC. The "force_new_file_options_dialog" option in the config.pro file needs to be enabled.

Jeff

 

[looslib]

Being a full time CAD administrator, the change from UG to Pro/E is dramatic as far as system preparatuion work is required.

Unigraphics is far easier to set up and customize than Pro/E.



"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli
CAD/CAM System Analyst
Ingersoll-Rand

 

[ohio30]

I know that you have an answer to your thread... If you use a table in your drawing formats to hold the text for the format it is much better. When the format is added to the drawing the table stays with the drawing until it is deleted. Even if you place another format on the drawing the previous table will remain on the drawing.
We use this technique for our revision blocks. The revision block header is on the format and then each row of revisions can be added using Table --> Modify row/col --> Add row. If the format is replaced with another format the previous revision block can be moved in to place, since it will remain with the drawing until the table is deleted.

 

[procadman2]

I'll add one more thing.
If you add tables on a drawing which are looking for parameters, ie: model_name, Designer, etc, when a dwg is started and the model lacks these parameters it will ask for a value for same. It will subsequently add the parameters to the model.

Barring this procedure create a mapkey which adds the required parameters and prompts for values.

procadman2
Proe Design & Admin
Mechanical & Aerospace

"You can't build a reputation on something you haven't done."
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