Beginner Help

[ptc-4339982]

Hi, I am totally new to Creo software and my company has just purchased Creo Parametric. I have been on a basics training course and also have plenty of experience from other 3D packages.

What I need is some tips on setting up part parameters such as title, mass, designer, date etc which appear as prompts to be entered when a new part or assembly is created then also on creating a series of drawings blanks/title blocks which will bring all this information in. Iv spent hours searching with little luck so far.

I would also like a couple of points clarifying, does Creo Parametric have an inbuilt screws, nuts, washer library? Can you run simple stress analysis in Creo Parametric?

Thanks in advance.

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[sschroeder]

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

[sschroeder]

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

[sschroeder]

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

[sschroeder]

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

[BrianMartin]

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

[ptc-4339982]

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

[BrianMartin · Accepted solution]

Hi Steve...

It's like you're at the tip of an iceberg that extends down to the bottom of the ocean.

Title blocks are a monumental pain in the neck. You have to create them using TABLES, not just lines. The parameters you wish to automatically populate the title block MUST be contained in table cells of they will not work. The trick here is mimicing your "original" title block using tables.

Most people create very simple tables... a few rows down and a few rows across. This limits the "look" of your title block. To really have complete control over your title block... and mimic the look of your original, you should export a DXF or IGES of your company's original title block. Use that to help you create a table in Creo to duplicate the look of your original artwork. The steps below give you a rough idea of what you're up against. After the slides we'll talk about mass, scale, revision level, and other issues. As always, click the images below to see a larger, more easy-to-read version...

The example above is only an example. The title block at my company actually uses a similar block to the one above but there are also OTHER tables on the drawing, too. We have about 4 different tables of information including a revision block, tolerance block, units of measure block, and other items. Not to mention we have several different bills of materials which also have to mesh seamlessly with the format to create a coherent look and feel to the drawings.

The task of creating templates, formats, and start parts is no small feat.

In your email, you mentioned several parameters you wanted in your models:

Title

Drawn By

Date Drawn

Mass

Material

Revision Level

Scale

For Title, consider that sometimes you'll want more than one line of text for a title. Wrapping the words so they consume multiple lines can be done... but many companies break up their titles into separate parameters (as in my example above) to eliminate the need for word wrapping or special relations which automatically break the title into smaller chunks.

For Mass, if you've set the density correctly - OR if you've used a well-defined material file, you can use &pro_mp_mass, a system-created parameter which contains the mass of the current model. There are some tricks to using this and some caveats but just knowing the parameter name helps get you started.

Material can be set using your material file (which you'll likely have to create). There are a few ways to do this... but the best is to create a parameter within the material file called "material_name" and assign a string value to it. You can have Creo automatically report the name of the material file itself using &ptc_material_name... but this is often not as useful as you'd think. Making a separate string parameter to hold the name of the material and housing this variable inside the material file is much, much better. You can access parameters from within a material file using the syntax material_param("parameter_name"). This is beyond what I can cover in one email but if you want to know how this works, I'll do a separate email about it.

Revision Level is best controlled directly from PTC's Product Data Management software (Windchill or Pro/INTRALINK) if you have them. If not, you'll need to create this as a regular string parameter. However, consider NOT keeping this parameter in the solid model. Consider making this a drawing parameter. Often well-intentioned administrators make this a solid model parameter hoping to tie the model and the drawing revisions together. My personal preference is to keep it in the drawing only. Unless you have a PDM system, keeping the revisions straight is going to be a MONSTER task... and this extra parameter will just end up being a source of confusion.

Scale can automatically be reported on the drawing using the &scale parameter without having to add a new parameter to the model.

I'm going to answer question #2 in the next response. This one is getting rather long!

Thanks!

-Brian

[BrianMartin]

... to continue...

You wanted to create a series of materials and colors such that when a material is applied or changed, the model color changes. This is possible. You can assign colors to materials in Creo (and Wildfire 5.) Look into the settings for both global_appearance_map and mat_assign_appearance. In Creo these options are hidden down inside the File>Options menus. The help files do a good job of explaning how to set up material-driven colors. Ask if you need further guidance.

My personal opinion is that the assigning of colors based on material is not very useful. Eventually the limited color selection will make your assemblies harder to decipher. Still, the option is there if you want it.

And finally, you asked: "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?" The answer is no. Therefore, to keep things straight without a PDM system, you have to carefully manage your documents. When you go to release a drawing, create backups (File>Backup) and save them to unique directories for safe keeping. Be aware though, once you've saved a file to a backup directory, Creo will save all new files to that backup directory! It's a critical flaw in the system in my opinion... it makes it very difficult to maintain any sort of control over your drawings. The PDM system is highly recommended to store your files, manage revisions, and prevent a massive buildup of data on your system.

Over time, you'll be left with a rat's nest of files that can be extremely difficult to sort out. If you can convince your IT people or management to invest in the minimal and cheapest PTC PDM system (Pro/INTRALINK), you'll save yourself tremendous headaches.

I know that was long... I hope it helped!

-Brian

[ptc-4339982]

Thanks again for the help. I agree about the whole iceberg analogy looking into this whole issue is opening a real can of worms at the moment.

At the moment our current working practice works along the following lines imagining that we have 2 job numbers 10.518 and 10.519.

1. Existing autocad drawings are all copied from job number 10.518 and all have the file/drawing name 10.518.001, 10.518.002 etc etc. They are all renamed 10.519.001, 10.519.002 etc and placed in the 10.519 job folder in a gen folder for working drawings.

2. As they are updated or altered to suit the new job the title blocks get updated with issue dates and issued by. Once they have been updated and finised they are copied to a fin folder and now final.

I think that these steps will fall down with Creo and drawing links will fail all over. It would mean having to open the assembly and replace all the items with the new numbers, which I can't seem to get to work at the moment. (Very time consuming and no better than where we are currently). I presume you will tell me that Windchill or Intralink are the only solution to this. Other than altering the way we manage files.

Going back to my initial questions I think I should be able to come up with something suitable based on your advice already. However thinking about it now on certain drawings we will currently have several materials listed i.e.

a) 150x50 RSA

b) 100x50 PFC etc

It would be better to keep this format seperate to a title block.