Creo Parametric Tips

May 24, 2024

Creo Parametric: Multibody Home -- Start Here! I'm creating this blog to be the central home page for anyone interested in trying out the new capabilities first introduced in Creo 7.0 that support multibody design. Below will be links to other blog posts on specific detailed topics under the general heading of multibody. I'm interested in getting your feedback on all the new stuff, but I also want to try to do this in a somewhat organized fashion. So, you can think of this blog as the top node of a tree that will have a number of branches below it for the various multibody related topics. In parallel to the list of blog posts below, I also plan to maintain a Multibody Infos post that provides you with links to further information, documentation, presentations, and any other information bits and pieces around multibody design in Creo. To get going effectively, I encourage you to first go through the What’s new material and tutorials that you find there, so that you have an overview and high level background on the use cases and capabilities. That will allow me then to go one level deeper and include some tips, tricks etc. in the blog posted here. I hope to be able to post new information regularly and hope you tune in, find it beneficial and give feedback in return. If you want to send me private messages, that’s fine, too. In particular if you have any suggestion on future blog post topics or questions, feel free to contact me at mneumueller@ptc.com . Enjoy…Martin Blog posts: Multibody – Intro, Model tree interaction and What’s that default body doing? Multibody- Seven 90sec-Tipps & Tricks around Booleans & Split Multibody - So many ways to trim a body Multibody - Creo 7.0.1 Enhancements Multibody - Windchill 12 & Creo 7.0.1 Multibody –How to display a body parameter in the model tree Multibody – How to display, use or call-out a body parameter – Part 1 Multibody - How to display, use or call-out a body parameter – Part 2 Multibody - Body selection, Body object vs Surface referencing Multibody - How to get rid of a body? - Show/Hide vs Remove Body vs Delete Body Multibody - How to save out a single body to .stl or step? Multibody - How does this all work with reference parts for MoldDesign and NC? Multibody - What are these Construction bodies? and all the details around them…. How to create a body intersection curve and what might it be good for? Multibody - How do I >position< bodies? Multibody - A simple body-based motion envelope cutout example Multibody - Clearance & Creepage Analysis Multibody - Model Tree Auto-locate capability: Update – Creo 7.0 vs Creo 8.0 & Creo 9.0 Multibody - External Copy Geometry (ECG) and body attribute propagation Multibody – A "Geometry Re-use"- Use Case that became possible with new capabilities in Creo 10.0 ..... And more to come…

May 18, 2020

Hello everyone and welcome to blog post #14 in this multibody blog series. Today’s blog is about the use of the “Intersect” Feature to create the intersection curve between two bodies (or quilts) You might remember that Creo 7.0 introduced Boolean Operations to perform merge, subtract and intersect operations between bodies. These operations act upon a “target” body which is modified during the Boolean operation. The resulting object there is still a body. In order to create an intersection curve, we therefore cannot use the Body Boolean operations feature, but will use the “Intersect” feature within the “Editing” group. Starting with Creo 7.0, this “Intersect” feature allows to select bodies as references. In this first example, we select Body 1 (yellow box) and Body (grey cylinder) and get the full intersection curve as a result. This is illustrated in the image below. (Result is shown in small overlay image) Note that you could also select just a single body in combination with one or multiple surfaces to get a partial intersection curve. In the example illustrated below we create the intersection curve based on a selection of the grey body 2 and 2 selected (red) surfaces of the yellow body 1. Finally, what could this intersection curve be used for? Intersection curves allow for a fast creation of a quilt representing the surface contours that are covered by the intersection (in particular for closed curves). You can for example use the curve generated in the first example as input to create a designated area. The image below shows the “Designated Area” feature with the closed intersection curve as input when placed on the yellow Body 1. The resulting quilt is illustrated in the small additional image. Starting with Creo 9.0 and higher you can also divide/split these surfaces based on those curves. Watch the video below to see an example use case of this. And as I was at video creation, I thought I could also re-emphasize the usage of Body visibility controls The usage of intent surfaces created by features such as “Divide Surface” and “Boolean Operations” Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo Parametric- Multibody Home: Start Here! Enjoy!....Martin

May 30, 2023

Hello everyone and welcome to blog post #20 in this multibody blog series. Today’s blog is about illustrating a use case around geometry re-use that became enabled with the new appearance (and reference) propagations in Creo 10.0’s Body Boolean and Split Body features. (see Multibody: Appearance and Reference Propagation for Boolean Operations (ptc.com) ) In essence we added two new options to Body Booleans as shown in the image below. Those options allow you to control color propagation and reference propagation. That means for the below example, that when you subtract the orange and white bodies from the green eyelet part, we can propagate the color to the corresponding mating cut faces, and transfer references from the original to the new surfaces, so that for the attached annotations automatically move to the cut surfaces. So, what is this good for? An example use case for this might be a scenario where you have standardized cut-outs for a connector where you model the cut-outs as fully detailed and annotated bodies in a library part. These bodies will then be inserted along with their annotations into the connector part where we then subtract and pattern them. During the subtract operation we can then not only create the target cut-out geometry, but also have the colors and the annotation references be transferred to the cut-out surfaces. All the sematic references of these annotations would thus continue to show in a semantic query for selected annotations. Here you see a video illustrating the workflow for the above example in Creo 10.0 Thanks for reading. I hope it was informative and this is a valuable use case for you. If you liked it, give it a Kudo. Back to Creo Parametric - Multibody Home: Start Here! Enjoy!....Martin

May 30, 2023

Hi all, as this came up in several threads, let me add a consolidated post here referring to External Copy Geometry (ECG) and body attribute propagation. The questions here are mostly related to the logic of the propagation options for bodies (and also other objects) Note that the ECG has settings within its option panel to control the propagation of parameters. This includes several aspects ranging from appearances to body names and more, and it also includes an option to propagate the construction body attribute. It also depends on whether an external body/or bodies are added "as is" or being merged into the existing body in the part. Here is how the options look like: Some questions had been raised for example about how the construction yes/no option works when a body is brought via ECG from a source model to a target model, initially with that option checked and then unchecked during Edit-Definition of the ECG. The answer to that is that this option is a logical toggle that allows to control whether the status/attribute from the source should be propagated to the target. If you "uncheck" it, the "construction" body attribute/status will no longer be propagated to the target. That means an update of the ECG will no longer force an update of the construction attribute in the target body. That means the target body will stay a construction body (simply because that is its current state and no update is forcing the body to change that status.) If you do a right-menu action on the body to "Unset construction body" status, then the body should become a regular solid body and should no longer change to construction during an ECG update. The publications team is currently working to provide additional explanations to the behavior into the online help sections. You should see that in the upcoming maintenance releases. Back to Creo 7.0/8.0++ Multibody Home: Start Here!

Sep 30, 2022

Multibody - Model Tree Auto-locate Capability Update – Creo 7.0 vs Creo 8.0 & Creo 9.0 Hello all, As I got a few comments & questions from time-to-time about the auto-locate functionality and its behavior, I wanted to shed some light on Auto-locate configurations and related changes between Creo 7.0, 8.0 and 9.0. What is auto-locate? Auto-locate is the capability to automatically find, show and highlight selected items in the tree. When you select geometry in the graphics, auto-locate will find the feature that created that geometry, expand nested tree hierarchy levels where required, and scroll the tree so you can see the tree node of that feature. When auto-locate was introduced, features were shown only once (e.g there was single node in the model tree representing the feature) and so there was no ambiguity as to which tree node instance of the feature to actually auto-locate to. #1) Creo 7.0: With the introduction of Multi-body in Creo 7.0, we introduced the Design Items folder that optionally allowed to list the bodies in the model along with their contributing features. This led to additional feature nodes showing up in the tree. ( Note: The display can be configured within the model tree filter settings) For Creo 7.0, the following options were available to control the body and body features display: Note that the option “Auto locate features in body sub-nodes” allowed to control whether a feature node should be located in the feature tree as it worked in the past or whether it should be auto-located underneath the body that it contributes geometry to (e.g. locating the feature node within the contributing features list of/underneath a body) #2) In Creo 8.0 we added more options, added the display of quilts and their contributing features in the Design Items Folder, and moved the auto-location option to a new place. It now resides together with all the other auto-locate and highlighting related tree options. To control the auto-locate behavior, you now need to go to the “Selection Priority” setting under the tree options and set it to “Feature List” or “Design Items”. As you can see in the screen shot, the round surface selection in the graphics triggers an auto-location to the feature node in the regular feature tree list and not within the Design Items as the setting is set to "Feature List". But there is additional flexibility: In a configuration where both trees are shown, you can now actually achieve a simultaneous auto-locate in the feature tree and Design Items tree side-by-side. #3) In Creo 9.0 (Beta) you will find the Selection Priority in that same place underneath the Tree Options within the tree's new toolbar. In addition you will find some additional auto location related enhancements once this version releases to the public. I hope that helps you to customize the tree display and the auto-locate behavior to your personal preferences and needs. Back to Creo 7.0/8.0++ Multibody Home: Start Here!

Mar 28, 2022

Multibody – Clearance & Creepage Analysis, Hello all and welcome to another blog post in the multibody series. In today’s topic I would like to make you aware of the multibody setup possibilities for clearance and creepage analysis. With the introduction of bodies in Creo Parametric 7.0, we also introduced support of the COMPARATIVE_TRACKING_INDEX parameter for bodies. If you add it to individual bodies of a part, you can define and control the conductivity definition separately for different bodies within a part. The attached video shows an example on a fuse part by defining conductive ends as body with a different CTI value. Once the body level parameter values are defined, you can see the conductive highlighting including the metallic ends of the fuse and excluding the red inner body. (view in My Videos) Thanks for reading & watching. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Jan 19, 2022

Nov 12, 2021

Hello all and welcome to another blog post in the multibody series. Today’s topic represents an add-on to the previous post : How to “position” a body. The workflow example in the below video explains in more detail how you can leverage these (previously discussed) positioning operations to create a design like this very easily. he intent here is to drive the cutout of the blue body parametrically based on the defined range of angular movement of the yellow pin. The workflow example makes use of the Flexible Modeling Move feature to create something like a “simplified motion envelope” driving the cutout opening in the blue body. (view in My Videos) Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Oct 12, 2021

Hello all and welcome to another blog post in this multibody blog series. Todays topic: How to “position” a body. You might wonder why I put the word position into quotes. The reason for this is that when we talk about positioning, many of us start thinking of positioning component-like objects. The fact that components have their system of reference (e.g. coordinate system including the origin) makes it natural to understand that positioning transforms that coordinate system from one location and orientation into another. Geometric bodies do represent a volume of geometry referring to the part’s reference system, therefore the positioning of geometric bodies should probably be better called “Moving” geometry. Anyway, after this introductory thought, I hope you enjoy the video illustrating how this is done in Creo. (and you won’t be surprised: we are going to use the “Move”-Feature for this workflow 😊) (view in My Videos) Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Oct 12, 2021

Hello all and welcome to another blog post in this multibody blog series. Todays topic: Construction bodies! Construction body are a pretty unique, powerful concept in Creo’s multibody implementation. As such it is really important to know about them and to understand how to use them. So, what are construction bodies? Construction bodies are bodies that are used for the design of your model, but do not contribute to the final geometry or mass. That means that similar on how you used quilts in the past to create additional geometry helping with the construction of your design, you can now do the very same with solid geometry. The construction attribute of these bodies will then help you to differentiate that geometry and automatically exclude it. Excluding them from mass properties is just one out of more than a dozen workflows where they are treated special. You will find more details in the video. (view in My Videos) Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Oct 12, 2021

Some Creo modules or applications such as NC or mold design modules do not yet fully support multibody models (as of Creo 7.0/8.0). Watch the below video to understand what you can do in these cases and how you can get to the required reference models for these downstream applications. Thanks for reading and many thanks to my colleague Beat Fretz who provided this example model (view in My Videos) to me. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Oct 12, 2021

Hello everyone and welcome to another blog post in this multibody blog series. This is a mini-post based on a question that I received: “If I have a designed a multibody model, how can I save out a single body to STEP , .STL or any other format?” The answer is pretty straightforward and involves either the remove-body feature (see blog post #10) or construction bodies (see blog post #13) or derived models (see blog post #12 and later). Method #1: Remove all other bodies using the remove-body feature Export(“Save A Copy”) the model to your desired format Undo the remove / delete the remove-body feature / suppress the remove-body feature Method #2: Set all other bodies to “Construction body” Invoke Export(“Save A Copy”) the model to your desired format Open the “Options”-menu in the “Save A Copy” dialog and ensure the Construction Body checkbox is unchecked Finishing the operation will then only save the remaining (non-construction) body The problem here might be that you need to remember which bodies to unset as construction afterwards if applicable Method #3: Create a derived model that only contains the body to be saved The easiest way to do this would be to select the body and then invoke “Create part from body” from the right mouse button menu. This creates a new part only containing the selected body allowing you to export it on its own Or Create new part and bring the desired body into the new part manually by using the “External Copy Geometry” feature (view in My Videos) Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0+ Multibody Home: Start Here! Enjoy!....Martin

Oct 11, 2021

(Remove a body versus hide a body vs delete body vs deleting/suppressing contributing features) Hello everyone and welcome to another blog post in this Creo multibody blog series. Today’s topic: Various way to “get rid of” a body and their differences Let’s have a look at various concepts that you might want to apply depending on what you want to achieve. Creo offers the following: Hide/Show a body As with other objects you can use show/hide commands to control the visibility of bodies. This is just changing the visual appearance toggling the display for a selected body and does neither remove the body object from the model, nor its geometry or mass “Consume a body” in Boolean features Boolean features have a Keep body option, to control whether the tool bodies should be consumed in the operation or whether a copy of their geometry should be used for the Boolean operation. Consumed bodies are shown in the body folder depending on the tree filter settings. “Remove body” feature This allows you to create a feature to consume a body. The body cannot be used further, and its geometry is removed. Note that the features are not removed or deleted but the geometry created by those features will not show anymore. Remove body is a feature so you can suppress or delete it or roll-back the model to before the Remove-Body feature to get the body back. Would suppressing contributing features also work to get rid of a body? This could potentially work in very simple examples for cases where these contributing features have no dependent children features and none of the contributing features contribute to or impact other bodies as well. In contrast to that, the remove-body feature leaves the other design features intact and just removes the body at time of its regeneration. Note that the body is still active and used in regeneration states before the remove-body feature. Good examples that illustrate the benefits and need for a remove body features (where suppressing features wouldn’t help or not be possible are: a situation where you bring several bodies A,B and C into a part via a single import feature or copy-geometry, or merge/inheritance feature and you want to only remove body B. a situation where you mirror a part design having bodies A,B and C to get A’, B’ and C’ and you just want to get rid of B’ Delete a body The delete body command completely deletes the body from the model for situations where you want to entirely get rid of the body object, free up its name in the name space and entirely remove it from the internal model entity data base. This is possible for two workflows: Delete new empty body Delete a body that doesn’t have any contributing features anymore (view in My Videos) Thanks for reading. I hope it was informative. If you liked it, give it a Kudo. Back to Creo 7.0 & 8.0 Multibody Home: Start Here! Enjoy!....Martin

Oct 11, 2021

During our B&W Webinar Week 2021, there are two sessions about " I spy with my little eye" which deal with the visibility of elements in Creo Parametric. In the first part of this two-part webinar we analyze the different tools and methods that Creo Parametric offers to make items visible or invisible in the graphics area. The organizational layer ‚Body‘, that came out with Creo 7 also impacts the visibility of items. The webinar especially focuses on: Visibility basics of objects and items in Creo Levels of visibility Differences in assemblies, parts and drawings Functionality to drive visibility Layers and layer states Combined states Simplified representations Style states In the second part of this webinar we will discuss some practical examples of the visibility topic and show the related tools and methods. Finally we will show how SMARTUpdate can help to implement and handle the techniques to drive visibility. Have a look at the recordings now: Part 1: (view in My Videos) Part 2: (view in My Videos) We hope you like it! Please feel free to ask questions here.

Oct 5, 2021

Welcome to Creo Coffee with a CAD Expert Series Registration link : https://www.ptc.com/en/technologies/cad/coffee-with-an-expert Main Presenters: Nicole Casalini (Application Expert) ,Gabriel Valls (Application Expert) and Guille Pezet(Application Expert) when : EVERY THURSDAY 11am CET / 10am BST Below you will find all the topicd and date for the webcast Date Topic Aug 19th Basics of Creo Modelling Aug 26th Manufacturing with Creo Sept 2nd Introduction to PLM Sept 9th Mathcad Sept 16th CAD for AR Sept 23rd What’s New in Creo 8 Sept 30th Ansys Partnership (Simulation)

Sep 17, 2021

Jul 26, 2021

Welcome to another multibody blog video in which I want to shed some light on body selection and when to reference body surfaces versus bodies as objects. The video covers: Body Selection Model tree Selection filter Query-Select & Pick from list Select quilt or body Select from parents Autolocate & Selection Priority in Creo 7.0 & Creo 8.0 Design Items tree Surface Selections RMB: surfaces of all bodies RMB: body surfaces Surface collection – Details dialog Geometry Search Differences Copy-Geom Pattern FMX Move (view in My Videos) Thanks for reading. I hope it was informative. Back to Creo 7.0 & 8.0 Multibody Home: Start Here! Enjoy!....Martin

Jul 26, 2021

Jul 9, 2021

Hello everyone and welcome back to the multibody blog series. This post also attempts to answer another body parameter related question: How can I display call-out a body parameter in a generic way? We received a question and enhancement idea from customers adopting Creo 7.0 asking for Leader Note Callouts for Bodies, similar to existing notations available for models, features etc as described in the Creo help here. (in short: Previously, when attaching a leader note to a model (component) you can get the value of a specific parameter for the attachment model. This can be achieved with the following syntax: &<param_name>:att_mdl e.g &BOM_PART_NO:att_mdl) An analogue workflow is now supported for body parameters. We implemented and added this to Creo 8.0. This enhancement allows you to call out the values of body parameters into a leader note that is attached to that body. To call out the value of a specific body parameter, you need to use the following syntax inside the leader note that is attached to that body: &<body-parameter-name>:att_body For example, if you have a body parameter called Description, you could create a leader note with the callout &Description:att_body or call out the body’s material using &PTC_ASSIGNED_MATERIAL:att_body When you create a leader note with this syntax, Creo Parametric checks the body to which the note leader is attached. If the called parameter exists for that body, then the body parameter gets evaluated and the parameter value is shown in the note. In the case of an assembly, Creo Parametric looks for the called parameter in the body of the component to which the note is attached. The callout is supported for all the environments and modes that already support :att_mdl. Example: All bodies have a DESCRIPTION parameter called out using &Description:att_body Thanks for reading. I hope it was informative. Back to Creo 7.0 & 8.0 Multibody Home: Start Here! Enjoy!....Martin

May 7, 2021

Hello everyone and welcome to blog post #7 in this multibody blog series. This post also attempts to answer another body parameter related question: How can I display, use or call-out a body parameter? If you want to call out a body parameter then you have to use the syntax as explained in the Creo help here. &<param_name>:BID_<body_feature_ID> Or &<param_name>:BID_<body_userdefined_name> Note: For bodies that have the default name (body 1, body 2, etc) you cannot use the system-defined default body name but you have to use the body’s Feature ID. (The reason is that the system-defined names such as body 1, body 2, etc are localized and translated into other languages and therefore not representing stable references across languages.) Example: Let’s assume we have 2 bodies. Here their names and parameters list. To call out the parameter “MY_BODY_INFO” for both bodies, we can now use the following for body 1 &MY_BODY_INFO:BID_-5778 And one of the following options for the WHEEL body (which has id 6105) &MY_BODY_INFO:BID_6105 &MY_BODY_INFO:BID_WHEEL So if you create a note and enter: You will see the resulting note text being: I think we have a preference of using body names. Therefore the system automatically tries to convert the body IDs to body names where possible. So when you go back to the call-out symbol definition, you will see it being changed to Thanks for reading. I hope it was informative. Back to Creo 7.0 Multibody Home: Start Here! Enjoy!....Martin

Oct 14, 2020

Creo Parametric Tips

Creo "What's New in Creo 11" Tips & Techniques Session Recording (West Coast)

Creo Parametric: Multibody Home -- Start Here!

Multibody - How to create a body intersection curve and what might it be good for?

Multibody – A Geometry Re-use Use Case that became possible with new capabilities in Creo 10.0

Multibody - External Copy Geometry (ECG) and body attribute propagation

Multibody - Model Tree Auto-locate Capability Update – Creo 7.0 vs Creo 8.0, Creo 9.0

Multibody – Clearance & Creepage Analysis

Plastic Part Design Tips & Techniques Session Recording (West Coast)

Multibody – FMX-Move: A simple body-based motion envelope cutout example

Multibody – How do I >position< bodies?

13. Multibody – What are these Construction bodies?

Multibody -12 How does this all work with reference parts for MoldDesign and NC?

Multibody - How to save out a single body to .stp, .stl?

Multibody - How to get rid of a body

Recording of "I spy with my little eye (Remastered) Part 1 and 2"

Coffee with a CAD Expert Series

Creo Multi-Body Design Tips & Techniques Session Recording (East Coast)

09 Multibody – Body selection, Body object vs Surface referencing

Creo Multi-Body Design Tips and Techniques Session Recording (West Coast)

Multibody - How to display, use or call-out a body parameter – Part 2 (new in Creo 8.0)

07 - Multibody – How to display, use or call-out a body parameter – Part 1

Creo Tips and Techniques Webcast Series (West)

Creo Tips & Techniques Webcast Series (East)