Beginner Help

Steve,

As you may know, you can setup parameters in a "start part" by creating a part and using the Tools, Parameters icon to create parameters. I typically just create description, alt part number (for vendor part), title for the drawing, and modeled by. There are some system parameters that you can leverage rather than creating new ones (like mass and date). For mass, change the pull down in the lower left of the parameters dialog box to "Reported Mass Properties". If it's 0, you'll need to assign a material and run a mass props report. You can do that in the File, Prepare, Model Properties dialog box. You can also have paremeters in the drawing only.

Once you create a "start part", you can place it in the default templates directory. For Creo 1.0, that directory should be something like C:\Program Files\PTC\Creo 1.0\Common Files\M010\templates. Once you place the file there, you can unselect the check box for "Use Default Template" when creating a new part. You should see your start part in the list. If you select on your part, then the parameters you defined should be shown in a list below. You can alter the default start part and other options using templates from the Configuration editor. Use the File, Options, Configuration Editor (in dialog box), and then search for "template". You'll see a number of options.

As for libraries, PTC does have a library CD you can download from www.ptc.com. It should be in the software download page. You may have to search the directory that contains Pro/E CDs for the "Basic Library" CD. Alternatively you can use a web site like the following: http://www.mcaduser.com/Portal/Models3d/05-Fasteners/fasteners.htm .

You can run simple linear static single part stress analysis with Creo Parametric. Your license should come with "Mechanica Lite". Select the Applications tab when a part is open and then select "Simulate".

Good Luck

Steve,

As you may know, you can setup parameters in a "start part" by creating a part and using the Tools, Parameters icon to create parameters. I typically just create description, alt part number (for vendor part), title for the drawing, and modeled by. There are some system parameters that you can leverage rather than creating new ones (like mass and date). For mass, change the pull down in the lower left of the parameters dialog box to "Reported Mass Properties". If it's 0, you'll need to assign a material and run a mass props report. You can do that in the File, Prepare, Model Properties dialog box. You can also have paremeters in the drawing only.

Once you create a "start part", you can place it in the default templates directory. For Creo 1.0, that directory should be something like C:\Program Files\PTC\Creo 1.0\Common Files\M010\templates. Once you place the file there, you can unselect the check box for "Use Default Template" when creating a new part. You should see your start part in the list. If you select on your part, then the parameters you defined should be shown in a list below. You can alter the default start part and other options using templates from the Configuration editor. Use the File, Options, Configuration Editor (in dialog box), and then search for "template". You'll see a number of options.

As for libraries, PTC does have a library CD you can download from www.ptc.com. It should be in the software download page. You may have to search the directory that contains Pro/E CDs for the "Basic Library" CD. Alternatively you can use a web site like the following: http://www.mcaduser.com/Portal/Models3d/05-Fasteners/fasteners.htm .

You can run simple linear static single part stress analysis with Creo Parametric. Your license should come with "Mechanica Lite". Select the Applications tab when a part is open and then select "Simulate".

Good Luck

Steve,

As you may know, you can setup parameters in a "start part" by creating a part and using the Tools, Parameters icon to create parameters. I typically just create description, alt part number (for vendor part), title for the drawing, and modeled by. There are some system parameters that you can leverage rather than creating new ones (like mass and date). For mass, change the pull down in the lower left of the parameters dialog box to "Reported Mass Properties". If it's 0, you'll need to assign a material and run a mass props report. You can do that in the File, Prepare, Model Properties dialog box. You can also have paremeters in the drawing only.

Once you create a "start part", you can place it in the default templates directory. For Creo 1.0, that directory should be something like C:\Program Files\PTC\Creo 1.0\Common Files\M010\templates. Once you place the file there, you can unselect the check box for "Use Default Template" when creating a new part. You should see your start part in the list. If you select on your part, then the parameters you defined should be shown in a list below. You can alter the default start part and other options using templates from the Configuration editor. Use the File, Options, Configuration Editor (in dialog box), and then search for "template". You'll see a number of options.

As for libraries, PTC does have a library CD you can download from www.ptc.com. It should be in the software download page. You may have to search the directory that contains Pro/E CDs for the "Basic Library" CD. Alternatively you can use a web site like the following: http://www.mcaduser.com/Portal/Models3d/05-Fasteners/fasteners.htm .

You can run simple linear static single part stress analysis with Creo Parametric. Your license should come with "Mechanica Lite". Select the Applications tab when a part is open and then select "Simulate".

Good Luck

Steve,

As you may know, you can setup parameters in a "start part" by creating a part and using the Tools, Parameters icon to create parameters. I typically just create description, alt part number (for vendor part), title for the drawing, and modeled by. There are some system parameters that you can leverage rather than creating new ones (like mass and date). For mass, change the pull down in the lower left of the parameters dialog box to "Reported Mass Properties". If it's 0, you'll need to assign a material and run a mass props report. You can do that in the File, Prepare, Model Properties dialog box. You can also have paremeters in the drawing only.

Once you create a "start part", you can place it in the default templates directory. For Creo 1.0, that directory should be something like C:\Program Files\PTC\Creo 1.0\Common Files\M010\templates. Once you place the file there, you can unselect the check box for "Use Default Template" when creating a new part. You should see your start part in the list. If you select on your part, then the parameters you defined should be shown in a list below. You can alter the default start part and other options using templates from the Configuration editor. Use the File, Options, Configuration Editor (in dialog box), and then search for "template". You'll see a number of options.

As for libraries, PTC does have a library CD you can download from www.ptc.com. It should be in the software download page. You may have to search the directory that contains Pro/E CDs for the "Basic Library" CD. Alternatively you can use a web site like the following: http://www.mcaduser.com/Portal/Models3d/05-Fasteners/fasteners.htm .

You can run simple linear static single part stress analysis with Creo Parametric. Your license should come with "Mechanica Lite". Select the Applications tab when a part is open and then select "Simulate".

Good Luck

Hi Steve...

Steve Schroeder answered the question about Mechanica Lite. he also mentioned the PTC library of fasteners. Most companies end up making their own version of a fastener library. One of the main reasons is the parameters you mentioned. Each company decides its own parameters... and the default Pro/E library doesn't incorporate them. Therefore you'll either have to modify the PTC library or make your own.

I believe you'll find the PTC basic library too simplistic for your needs. It may work in a pinch but those libraries rarely differentiate between thread sizes and other factors you'll likely require from your library. They're literally just basic geometry to represent a fastener.

Deciding upon relevant parameters and setting them up to work properly is not an insignificant task. To be honest, it's a bit of a pain in the neck. Mr. Schroeder mentioned a few suggestions but each company really needs to decide on it's own.

After having configured parameters, templates, and formats at many different companies, my best advice is KEEP IT SIMPLE. While you may be tempted to add a whole host of parameters in hopes of "automatically filling out the drawing", I'd advise against it. For example, many companies use a drawing format that incorporates an approval block. Several reviewers or engineers are expected to sign off on the drawing before it can be approved for release. Having a parameter for each approver's name and date is tempting. Theoretically you could edit these parameters in your models and never have to mess with them in your drawing. this plan never quite works as well as you'd think. It's always a bigger mess than it should be.

The discussion on the "best way" to set up your models and drawings is quite a bit beyond what I could cover in one message. There are nuances that make this more of an art form than a science. There are multiple issues that come into play:

• Parameters can be stored inside the solid models (parts and assemblies). They can then be displayed on the drawing. However, parameters can also exist solely in the drawing without being tied to a specific model. There are very good reasons to use both types. (I can elaborate if you need more information).
• Standard parts, assemblies, and sheet metal parts can all have templates which are called upon when starting a new part, assembly, or sheet metal part. As the other Steve said, these are called "start parts". They can also incorporate standard views, layers, colors, materials, units, and other pertinent features.
• Drawings are a major source of customization at each company. You'll need to design formats to suit your needs. You'll also need to decide which information should appear on Bills of Materials. This ties in directly with your choice of parameters (and possibly your materials) in your solid models. Drawing formats can "pull" parameters from the models (OR from internal parameters saved within the drawing) and display them anywhere on the field of the drawing.
• Special configuration options (accessed through the File>Options menu in Creo Parametric 1.0) control a host of issues related to drawings, formats, parameters, and start parts. This is just a partial list of settings to be concerned with:
  • make_parameters_from_fmt_tables
  • todays_date_note_format
  • drawing_setup_file
  • format_setup_file
  • template_designasm
  • template_drawing
  • template_sheetmetalpart
  • template_solidpart
• Developing a good Materials library is crucial if you wish to use or calculate mass properties for your models. TYou can create as many materials as you wish... each has a separate file to control all aspects of the material. There are special parameters you can set in these files which will report back to your models and drawings. This data can be represented in a drawing format or bill of material, too. The process for this isn't always easy.
• Drawings can also have template files. These drawing templates can pre-place views on the field of your drawing. They can also pre-load symbols, notes, and other useful information to automate drawing creation. Drawing templates are different than drawing formats. Formats provide a basic framework... templates begin to fill out that framework with additional information.

It's difficult to give much more information without understanding more about your drawing formats, bills of materials, and what type of components your company will be working on. There are so many other threads of discussion that feed into your question... such as data management (how are you managing and storing the data you create in Creo Parametric?). If you can ask some specific questions or give a bit more guidance, I can help direct you to further information. It's tough to talk in generalities when this topic really requires more details to get you going.

Write back with details about your models, formats, and what you'd like to accomplish. I'll try to point you in the right direction. The information PTC provides on these topics is hard to digest for new users.

Thanks!

-Brian

Thanks for the advice. I have managed to get some models underway with some parameters setup based on your suggestions.

The parts I will be modelling will cover simple angle brackets, simple ducting, simple steel section frames up to more complex large section frames, flat sheet and simple rollers. We would like our current title blocks format to be carried into Creo and these include:-

Title

Drawn By

Date Drawn

Mass

Material

Revision Level

Scale

I would like the designer to fill these fields in when he draws the models/assemblies and have them brought through into the title block when he creates the drawing.

My initial tasks and requirements are:-

1. To create a series of title blocks which include this information above automatically. (Is creating a title block simple a case of sketching fields/boxes and adding references to parameters?).
2. Create a series of materials and apply colours to them so that when the designer applies a material the colour changes or is brought up to apply the changes.

Another little issue is Creo creating previous versions of files, is there a way to set a seperate directory for these rather than into my working drawings directory?

I may have more later but this would be a great start.

Thanks