Creo Engineering Notebook Tips n' Techniques

Overview

This 57-minute PTC Tips & Techniques webcast, presented by Anji Seberino (SME Field Director) and moderated by Tom Quaglia (Creo Solutions Consultant), shows how to use Creo Engineering Notebook powered by Mathcad to keep engineering calculations inside a Creo model and use them to drive geometry. It is aimed at Creo Parametric users who do design calculations in Excel, Word, or standalone Mathcad today. It includes a live gear-design demo and a Q&A on Excel data, units, Windchill, iteration, and supported data types.

Chapters

This video has chapters, also available from the player menu.

• 0:00 to 4:12: Welcome and PTC User Global Summit key dates
• 4:12 to 9:14: What is Creo Engineering Notebook powered by Mathcad?
• 9:14 to 11:02: Why use it: document, calculate, optimize, validate
• 11:02 to 13:19: Engineering Notebook vs standalone PTC Mathcad
• 13:19 to 17:26: Gear demo: opening the embedded notebook
• 17:26 to 22:40: Inputs, outputs, and live calculations
• 22:40 to 27:43: Save and Push to Creo, and why you regenerate twice
• 27:43 to 31:34: Driving the notebook from a Creo parameter
• 31:34 to 33:09: Q&A: tolerance stack-ups and Creo EZ Tolerance Analysis
• 33:09 to 39:56: Reading and writing Excel data
• 39:56 to 43:40: Units: rescaling values before sending to Creo
• 43:40 to 48:30: Q&A: Windchill, data types, measurements, iteration
• 48:30 to 51:02: The Unit Sensitive checkbox in Creo relations
• 51:02 to 53:51: Applications tab vs Analysis tab, and user polls
• 53:51 to 57:51: Include, exporting, and renaming outputs

Key Takeaways

• Creo Engineering Notebook is installed, licensed, and launched from Creo, and its worksheets are saved inside the Creo model. PTC Mathcad is a separate standalone application, and both can be installed on the same machine with no conflict.
• Data flows both ways: Creo parameters can feed the worksheet as inputs, and worksheet values tagged as outputs on the Input/Output tab are pushed back to drive the model.
• After you Save and Push, regenerate the Creo model twice. The first regeneration syncs the data, and the second updates the geometry.
• Only Creo parameters can be passed to the notebook. To use a measurement, save it as a feature and create parameters from that feature.
• Windchill sees a Creo model with an embedded notebook as one object. There is no separate worksheet file.
• To send a value to Creo in different units, divide it by the desired unit in Mathcad before tagging it as an output. The Unit Sensitive checkbox in Creo relations only works within the same base unit.
• Engineering Notebook lives on the Applications tab. Mathcad Analysis and Prime Analysis on the Analysis tab work differently and do not embed a notebook in the model.

What is Creo Engineering Notebook powered by Mathcad?

Creo Engineering Notebook powered by Mathcad is a digital engineering notebook embedded inside a Creo model, where you write math, text, assumptions, and decisions and run live calculations whose results can update the model. It combines the roles engineers often split across Word, Excel, and PowerPoint with the Mathcad calculation engine, which shows all math in natural math notation. When a notebook is embedded, a glyph appears in the top right corner of the model, and the worksheet is opened, edited, and saved within Creo.

Watch: 4:12 to 9:14 (slides showing a Mathcad calculation sheet and a crankshaft assembly with an embedded notebook)

Why use Creo Engineering Notebook instead of Excel for design calculations?

Creo Engineering Notebook keeps your calculations, methods, assumptions, and decisions with the Creo data, so you and your colleagues can open the part or assembly later and see the thought process behind it. Beyond documentation, the calculations can drive dimensions, explore what-if scenarios and variations, optimize a design against constraints and objective functions, and validate the design. Values move in both directions between the notebook and the model.

Watch: 9:14 to 11:02 (slide summarizing the reasons to use Engineering Notebook)

How is Creo Engineering Notebook different from PTC Mathcad?

Creo Engineering Notebook is a Creo capability, while PTC Mathcad is a standalone application, even though both are powered by Mathcad. Creo Engineering Notebook is installed through an opt-in option in the Creo installer, licensed from Creo, launched from Creo, and its worksheets are saved with the Creo data. PTC Mathcad is installed, licensed, and launched independently, and its worksheets are saved separately. You can run both: use Engineering Notebook for calculations tied to a Creo design, and PTC Mathcad for calculations outside Creo.

Watch: 11:02 to 13:19 (side-by-side comparison slide of the two products)

How do I add or open an Engineering Notebook in a Creo part?

You add and open Creo Engineering Notebook from the Applications tab in Creo, and once a notebook is embedded you open it by clicking its glyph in the upper right corner of the model. From the Applications tab you can also insert a Mathcad worksheet you created earlier, or remove the notebook. The demo uses a gear part with a 12-page notebook that combines gear-design background, graphics, terms, and definitions before the calculations start on page five.

1. Open the Applications tab: Select Engineering Notebook.
2. Add or insert a worksheet: Add a new notebook, or insert an existing Mathcad worksheet.
3. Open the notebook: Click the glyph in the upper right corner of the model. An icon next to the worksheet name shows that it is embedded in Creo.

Watch: 13:19 to 17:26 (gear part with addendum, dedendum, and pitch circles, then opening the embedded notebook)

How do inputs and outputs work in a Creo Engineering Notebook worksheet?

Inputs are values that come from Creo parameters and cannot be edited in the worksheet, and outputs are worksheet values you tag on the Input/Output tab so they are sent to Creo. The worksheet calculates from top to bottom and left to right, so changing a definition, such as the pressure angle from 20 degrees to 14.5 degrees, updates everything that depends on it. The gear demo also uses a dropdown for the module, if statements for conditional logic, a pass or fail check that the number of teeth is less than 20, and plots. Five values are tagged as outputs, including the number of teeth, the tooth thickness, and circle diameters.

1. Select the value: Select the calculated value in the worksheet that should drive the model.
2. Tag it as an output: On the Input/Output tab, assign it as an output.

Watch: 17:26 to 22:40 (scrolling through the gear calculations, conditional logic, plots, and the tagged outputs)

How do I push Engineering Notebook results to the Creo model?

Change the inputs in the notebook, use Save and Push to send the outputs to Creo, and then regenerate the Creo model twice. The first regeneration syncs the data between the model and the notebook, and the second applies the new dimensions to the geometry. You can also save without pushing while you explore options. In the demo, changing the module from 10 to 16 gives a gear with nine teeth, and changing it to 12 gives twelve teeth with a tooth thickness of 54.

1. Change an input: For example, change the module. Type a page number in the page box to jump straight to a page instead of scrolling.
2. Check the outputs: Confirm the results and the pass or fail check.
3. Save and Push: Use Save and Push to save the worksheet and push the outputs to Creo.
4. Regenerate twice: Regenerate once to sync, and again to update the geometry.

Watch: 22:40 to 27:43 (two design iterations and the gear updating with more teeth in a Creo table of outputs)

What happens when I change a Creo parameter that the notebook uses?

When you change a Creo parameter that the notebook uses as an input and regenerate, Creo shows a notification that the embedded notebook is out of date, and you update the inputs in the notebook before pushing results back. Change the parameter at the part level in the Parameters dialog, because values listed under the embedded Mathcad entry are locked. In the demo, the gear diameter D is changed to 125.

1. Change the parameter: Select Tools, then Parameters, stay at the part level, and change the value.
2. Regenerate: Creo notifies you that the embedded notebook is out of date.
3. Update the inputs: Open the notebook and update the inputs to pull in the new Creo value.
4. Push and regenerate: Save and Push, then regenerate the model.

Watch: 27:43 to 31:34 (changing the diameter parameter, the out-of-date notification, and the redesigned gear)

Can Creo Engineering Notebook do tolerance stack-ups?

Creo Engineering Notebook can do tolerance stack-ups, but Creo EZ Tolerance Analysis is a purpose-built tool for them. It is integrated in Creo, more graphical, and uses dimensions directly from the CAD model. Engineering Notebook can handle almost anything you do in Excel today, but in this case a dedicated tool already exists.

Watch: 31:34 to 33:09 (answer from the live Q&A)

How do I read and write Excel data in Creo Engineering Notebook?

Read Excel data with the Read Excel button on the Input/Output tab, which opens a wizard, and write Excel data with the Write Excel function under Functions, then File Access, which has no button. After reading, assign the result to a variable and extract the columns or single values you need. Indexes are zero-based by default, so the left column is column 0, and you can change this to one-based.

1. Read the file: On the Input/Output tab, select Read Excel and browse to the file.
2. Choose the data: Preview the data, pick the sheet, rows, and columns, then select Insert and assign the function result to a variable.
3. Check the data: Use the built-in rows and cols functions, or type the variable name followed by an equals sign to display it.
4. Extract values: On the Matrices and Tables tab, extract a column, or extract one element by row index and column index.
5. Send it to Creo: Assign the value to a variable, tag it as an output, and connect it to Creo.
6. Write back to Excel: Under Functions, then File Access, use Write Excel and give it the destination file, the data, and the location to write to.

If regions run off the page, landscape orientation gives you more width.

Watch: 33:09 to 39:56 (Read Excel wizard, extracting a single cell value, and finding Write Excel)

How do I handle different units between Mathcad and Creo?

If the worksheet and the Creo model use different units, divide the value by the desired unit in Mathcad and tag that result as the output. Mathcad stores values internally in SI units, so 11.5 inches is sent as about 0.29 meters unless you rescale it. The Unit Sensitive checkbox in Creo relations, found under Tools, then Relations, then Utilities, converts the value only when both sides share the same base unit, such as meters, centimeters, millimeters, and micrometers. If the base units differ, the checkbox has no effect and you must rescale in Mathcad.

Watch: 39:56 to 43:40 and 48:30 to 51:02 (rescaling 11.5 inches to millimeters, then the Unit Sensitive checkbox)

Can Engineering Notebook and Creo geometry exchange values in a loop?

Yes, Creo Engineering Notebook is not limited to a one-time, one-direction push, so you can iterate between calculations and geometry. For example, after the notebook drives the gear geometry, a Creo volume parameter can be sent back to the notebook, checked against design specifications, and used to calculate a second set of design values. Tom Quaglia noted that this overlaps with behavioral modeling but involves less syntax and documents the math better.

Watch: 46:13 to 48:30 (answer from the live Q&A)

Is Mathcad Analysis on the Creo Analysis tab the same as Engineering Notebook?

No, Mathcad Analysis and Prime Analysis on the Creo Analysis tab work in a completely different way and do not embed an engineering notebook inside the Creo model. To use Creo Engineering Notebook, start from the Applications tab.

Watch: 51:12 to 52:08 (presenter clarification with both tabs shown)

How do I reference another Mathcad worksheet from an Engineering Notebook?

Use Include on the Input/Output tab and browse to the other Mathcad worksheet, and its stored values and function definitions become available from that point forward in your notebook. Many users miss this because it is called Include rather than reference. It works much like reading in an Excel file.

Watch: 53:51 to 55:46 (adding an Include region at the end of the notebook)

Frequently Asked Questions

Q: Does Windchill store an embedded Engineering Notebook as a separate file?

A: No. Windchill sees the Creo model and its embedded notebook as one object, because the notebook is part of the Creo data. (answered at 43:40)

Q: Can I pass strings between Creo and Engineering Notebook?

A: No, not at the time of the recording. Strings cannot be passed back and forth between Creo and Mathcad. (answered at 52:39)

Q: Can I pass a Creo measurement into the notebook, or does it have to be a parameter?

A: It has to be a parameter, because everything goes through Creo parameters. If you save the measurement as a feature, you can create parameters from that feature and pass them in. (answered at 45:00)

Q: Can Engineering Notebook read Creo View PVZ files?

A: No. Engineering Notebook is integrated with Creo Parametric, not with Creo View. (answered at 45:41)

Q: Can I export an embedded notebook to an external Mathcad file?

A: Yes. (answered at 55:46)

Q: Can I rename notebook outputs to something meaningful instead of out_1 and out_2?

A: Yes. Select Show as List to open a table of the outputs. The names in the left column stay fixed and follow the order the outputs are tagged in the worksheet, but you can rename the aliases in the right column, for example to Addendum Diameter. (answered at 56:05)

Links & Resources

• Creo Engineering Notebook (ptc.com)
• Welcome to Engineering Notebook (Help Center) (support.ptc.com)
• Engineering Notebook in Creo (What's New: Creo Parametric 12.4.0.0) (support.ptc.com)
• Creo EZ Tolerance Analysis Extension (ptc.com)