Creo Parametric Tips

Hello Multibody community! As I recently have received some questions and suggestions around how to trim a body, let me spend a few minutes today to tackle that topic. #1) How can I trim a body by a datum, surface, quilt etc? I have heard this question several times, as there is no “Trim Body” tool currently in Creo Parametric 7.0. Still, we do have other tools that you can use to trim body geometry. If you want to trim a body by a datum, surface, quilt, this is the “Solidify-Tool” with the “Remove Geometry” option. Here are two examples how that would look like. Two hints if you want to try it: Set the body that you want to trim as default body. This saves you from needing to access the body options panel in the feature Pick the trimming object first to get access to the solidify feature #2) How can I trim a body by another body? This is often useful to perform Boolean operations with a trimmed “modifying body”. Here is an example of that where you might want to trim a “library-type”/”standard-type” grey tool body to only merge its upper half to the yellow plastic part. The most robust flavor of this might involve body split and body remove, but there are actually several more workflow flavors on how to achieve the above with mostly 3 steps. If you are interested in seeing all of different ways to achieve the result, watch a quick 6mins movie of that here: (view in My Videos) Back to Creo 7.0 Multibody Home: Start Here! Enjoy!....Martin

Jun 22, 2020

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 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 Multibody community! Welcome to a second post on multibody capabilities added in Creo 7.0.1. What I had not yet been fully covering in the last post was how Creo & Windchill interact as it relates to the multibody concept. So, here a summary of Multibody support for Windchill & Visualization General behavior Multibody parts are managed similarly to single body parts, bodies are not exposed Windchill versions prior to Windchill 12 Body designation information is ignored when connected to a Windchill Server version not supporting body designation yet Publishing of multibody parts to Creo View is supported since Creo View 6.1 (including exposure of bodies to Creo View) Windchill 12 & Creo 7.0.1 Support of Body designation, including Transfer of Body designation information from Creo to Windchill for models containing designated bodies WT part creation for designated bodies if BOM Designation is set (.prt, .asm) IBA mapping & propagation for body materials and mass property parameters Note on Windchill configuration: those attributes have to be added to the Body (under Model Items) type definition. They need to be part of the type definition similar as typically being done for the CAD Document type. Here is a quick demo of the above capabilities (view in My Videos) Back to Creo 7.0 Multibody Home: Start Here! Enjoy!....Martin

Sep 22, 2020

Hello Multibody community! Welcome to this new post on the multibody capabilities that we introduced with Creo 7.0. Meanwhile, the first maintenance release Creo 7.0.1 had been released and it does contain several refinements/enhancements to the initial set of capabilities. Here a list of those enhancements: Boolean Operations In Creo 7.0, the “Keep bodies” option in Boolean Merge, Subtract and Intersect features was only available during feature creation. Now it is also enabled during feature Edit-Definition workflows Curve feature You can now select a body (in addition to the previously available object types Quilt and Surface) when checking the “Place curve on surface” option. Data Exchange The “Import multiple bodies into one part” option is now available in File/Open (Unite) and ATB-enabled Import workflows Improved Body Handling Improved body handling when a feature-owned body (e.g. a body created by split-body, import or data sharing features) gets deleted from the model Data Sharing and Reference Pattern robustness enhancements for specific multibody situations Aligned Material reporting The mass properties report uses the parameter PTC_REPORTED_MATERIAL in all places where material is reported. New configuration option for multi-material parts: ptc_reported_material_mp_report Windchill support for designated bodies If you are interested in seeing demos of the above capabilities 1)-6), take 15mins to watch me walking through them. Beyond the new capabilities you might also find some of the multibody concept related background information useful. (view in My Videos) Note that I plan a dedicated video showing the Multibody related Windchill interaction for my next post. Back to Creo 7.0 Multibody Home: Start Here! Enjoy!....Martin

Sep 7, 2020

Jul 9, 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

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

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 #6 in this multibody blog series. I got asked recently : How can I display a user-defined body parameter in the model tree? If you are interested in that as well, here is how you do it. Let’s walk through an example step-by-step. Step 1) Let’s assign a body parameter (and let’s call it for example “MY_BODY_PARAM”) Step 2) Open the Model Tree Columns display dialog Step 3) Select the Type: Body Params Step 4) You might notice that the list shows system parameters related to bodies (e.g. PTC_ASSIGNED_MATERIAL), but not the newly added user-defined parameter Step 5) Manually enter the user-defined-parameter (in our example “MY_BODY_PARAM”) into the Name field and click the double-arrow to move it into the displayed columns Step 6) Click “OK” and ensure model tree columns are displayed. Now you should be able to see your body parameters as part of the displayed model tree columns q.e.d. 🙂 I hope that helped. Back to Creo 7.0 Multibody Home: Start Here! Enjoy!....Martin

Oct 14, 2020

(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

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

Blog Post 01 - I wrote a blog post about the topic of Multibody – Intro, Model tree interaction and What’s that default body doing? I figured it made sense to provide a more thorough explanation that would attempt to answer all the questions likely to come up. Check it out and if you have any additional questions/comments, add them under the blog post itself. Thanks! Martin (view in My Videos) Back to Creo 7.0 Multibody Home: Start Here!

May 18, 2020

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

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

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

May 29, 2020

Nov 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

Multibody Info – Collection Creo 7.0 - What’s new: Multibody Design Creo 7.0 – Multibody Tutorials (7 tutorials around multibody use cases including demo models, step by step instructions, videos and more etc) Creo Multi-Body @ Creo 7.0 PTC Virtual Conference – Includes a Multibody Use Cases & Benefits overview presentation Liveworx 2020 presentation Creo 7.0 Product Update Multibody Design - recording Liveworx 2020 presentation Creo 7.0 Product Update Multibody Design - slides Liveworx 2020 presentation Creo 7.0 Multibody Design - youtube CAD Conference October 2021 - Multibody Tipps & Tricks / Adoption / What to watch out for (replay) More to come Back to the main blog Creo 7.0/8.0+ Multibody Home: Start Here!

May 18, 2020

Creo Parametric Tips

03 - Multibody – Many ways to trim a body

Creo Parametric: Multibody Home -- Start Here!

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

05 - Multibody - Windchill 12 & Creo 7.0.1

04 - Multibody – Creo 7.0.1 enhancements

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

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

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

09 Multibody – Body selection, Body object vs Surface referencing

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

06 - Multibody –How to display a body parameter in the model tree

Multibody - How to get rid of a body

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

01- Multibody – Intro, Model tree interaction and What’s that default body doing?

Multibody – How do I >position< bodies?

Coffee with a CAD Expert Series

Multibody – Clearance & Creepage Analysis

02 - Multibody – 7x 90seconds Tipps & Tricks around Booleans & Split

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

13. Multibody – What are these Construction bodies?

Multibody Info – Collection

Creo Tips and Techniques Webcast Series (West)

Creo Tips & Techniques Webcast Series (East)