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Posted by Rand 3D on 09/14/2020 at 04:41 PM in CATIA, Creo, Industry News, PLM, Promotions, Tips and Tricks, Webcasts | Permalink
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Question 1: Is that "Create DFS option" new since Creo 5?
Answer to Question 1:
The Datum Feature Symbol command was introduced in Creo Parametric 4.0. In releases before Creo Parametric 4.0, a Set Datum was used.
Question 2: How many differences are there for Legacy Datums between Creo 3.0 and 4.0?
Answer to Question 2:
In Creo Parametric 3.0 (and earlier versions), a Set Datum was created as a property of a plane or axis feature. These referenced were either selected from existing references or created in the drawing.
In Creo Parametric 4.0 (and later versions), a Datum Feature Symbol is created as either a standalone annotation or inside of an annotation feature.
Question 3:
It appears you were able to add DFS to the model, why didn't you show annotations in the drawing?
Answer to Question 3:
Ideally, I would show the annotations in the drawing. What I wanted to demonstrate in the presentation is that you can add a datum feature symbol to the model or in the drawing.
Question 4:
If a DFS is created in Drawing mode, do they exist only in the drawing, or will it also exist in the model? Does it matter which mode it's created in?
What are the impacts of not converting?
Answer to Question 4:
A DFS (datum feature symbol) created in Drawing mode exists only in the drawing; it will not exist in the model. If you want the flexibility of changing the references to affect both the model and the drawing, create the DFS in the model.
The impact of not converting to DFS in Creo 4.0 (and later versions) is that if you need to make changes to dimensions or geometric tolerances, you will first have to associate the dimension or geometric tolerance to model geometry, which is why we need to create a datum feature symbol. Also, the older method of using set datums is based off of outdated standards. You will be required to convert legacy datums to comply with the latest design standards.
Question 5:
In Creo 4.0 why would the rotate datum be grayed out?
Answer to Question 5:
If we are referring to the button in the Additional Text group of the Datum Feature tab, you must enter text in the text field (make sure to hit <enter> key afterwards) in order for the button to highlight as shown.
Question 6:
How do you attach the DFS to a feature dimension in the model?
Answer to Question 6:
You just select the dimension to attach the DFS to. Once to select the dimension, you can move the frame to a desired location.
Question 7:
I'm new to Creo, why does it seem so difficult for such an easy operation?
Answer to Question 7:
A great question. I will say that as with most operations in Creo, there is a process. The process typically does not change much between versions. As the basic concepts are more important than the commands required to perform a task, in time you will be more comfortable with the process.
Question 8:
How do you get the dimension to show up?
Answer to Question 8:
I am not sure of the context, but you can show dimensions in the drawing using Show Annotations option.
And you can display dimension in the model tree by selecting (Settings) > Tree Filters > and check Annotations option.
Question 9:
I think they was already stated but I wanted to confirm. If I am using an older drawing that uses ASME Y14.5 1994 per the drawing, will I have to use a CREO version prior to 4.0 in order to edit any of the datums or to create new GDT off of the legacy datums?
Answer to Question 9:
If you are using an older drawing that uses ASME Y14.5 1994 AND you need to edit this drawing in Creo 4.0 (or later version), you will need to open the model in the Creo 4.0 (or later version) and convert the existing set datums to datum feature symbol annotations.
Question 10:
On a drawing I made recently, I got a duplicate datum name error. But the way we do our drawings I need the ability to have datums A, B, and C in multiple parts shown on the same drawing in order for the tolerance notes to make sense. Is that error message telling me that I have multiple datum C symbols on a particular part (which is something I don't want and thus is a useful error message) or is it warning me that I have multiple datum C symbols per drawing (and if that's the case is there a way to disable that warning?).
Answer to Question 10:
The following is the response from the attendee who asked the above question:
I figured out a work-around: by creating the DFS’s in the part instead of in the drawing (the key step I was missing was showing the dimension annotations in the part so that I could then select them when placing the DFS), I was able to create a separate datum C symbol on each part and then show them on the drawing annotations without it complaining. So it does allow multiple datum C’s, one for each part, as desired. My mistake was I expected incorrectly that when I created the datum feature symbol in the drawing attached to a part dimension that it would become a symbol associated with the part. But it was associated with the drawing view, not the part, and thus CREO was somewhat justified in its complaint that I had two datum C’s because they were both tied to the drawing (in their respective views), not to the parts.
Question 11:
In the newer style (Creo 4.0+), how are datum extension lines controlled/edited? They are currently displaying with a dashed line, and it needs to be a solid extension line.
Answer to Question 11:
Try setting the detail option leader_extension_font to SOLIDFONT.
Question 12:
Do the drawing mode options work if a combined state was used to create the drawing view?
Answer to Question 12:
Yes.
Question 13:
I do not see my draft datum created in the drawing in the model tree under annotations. I am using CREO 4.0 is there a specific way for the draft datum to appear the model tree on the part? Or does that only appear for legacy datums and not ones created in 4.0?
Answer to Question 13:
Draft datums do not appear in the model tree or in the part. In Creo Parametric 4.0, if the Annotate tab is active, draft datums will appear in the Drawing Tree under the Datums area ( ). If the Annotate tab is not active, you will not see annotations in the tree, though they are visible on the drawing.
If you want datums do not appear in the model tree, create the datum in the model. Then later when you are in the drawing, you will see that datum in the model tree. And you will be able to show the datum in the drawing using the (Show Model Annotations) option.
Question 14: Can we step through an example of troubleshooting a set datum that is placed on a datum axis that is at an angle/normal to current orientation plane?
Answer to Question 14:
This question will be addressed in a future blog.
Posted by Natasha Reaves on 06/01/2020 at 04:35 PM in Creo, Tips and Tricks, Webcasts | Permalink
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By Trisha Freeman
Thank you to everyone who joined us live for the Getting the most out of CATIA V5 FT&A (Functional Tolerancing & Annotation) Captures in a digital world webcast. The topics presented in the webcast can be further understood by attending the Functional Tolerancing and Annotation class with Rand 3D. If you would like to review the webcast again, or you did not have a chance to view it live, you can access the recording below:
To summarize, we spent some time talking about the advantages of using an FTA capture and how you can incorporate the annotation data for each view while being able to control other custom aspects such as establishing camera viewpoints, applying annotation filters, creating clipping views, and managing parts visibility.
Establishing a saved camera viewpoint can be done with the “Named Views” icon, and then use this saved view when creating a capture.
When creating a capture for a particular view, you can use the apply filter command to have only those relevant annotations be saved to the capture. First, double click on the capture in the tree to activate the capture creation area.
If a particular capture is mean to section a model then you must activate the clipping plane icon in the capture creation area.
Finally, if you are wanting to have certain geometrical sets, part bodies, or parts within a product to be able to be visible or hidden for captures, then you must activate this capability in the internal options.
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Here are the questions that were asked after the webcast last week, along with my answers:
Q: When you changed the material on the section view (change the hatching pattern of aluminum for example within a part file), were the changes applied for this part or it applied also to the material library?
A: It does not change the hatching pattern in the material library.
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Q: Is the FTA license required to simply view the annotations and do the annotations translate to other files like Step?
A: The FTA license is only required if you are creating or modifying annotation data. There are various configurations of licenses that will allow you to view annotation data (just remember to only right click and display the capture, do not double click on the capture because then it thinks you are trying to modify the data instead of simply viewing it). The annotation data can translate to step files, but you must make some additional changes in the internal options. Check out this blog for more details on how to export step files in CATIA V5.
Posted by Rand 3D on 06/03/2019 at 03:05 PM in CATIA, Webcasts | Permalink
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By Mike Brucker
Thank you to everyone who joined us live for the brief Introduction to Creo Parametric Behavioral Modeling webcast. The topics presented in the webcast can be further understood by attending the Creo Parametric Behavioral Modeling course with Rand 3D. If you would like to review the webcast again, or you did not have a chance to view it live, you can access it here.
The webcast taught us how to use the Creo Behavioral Modeling extension to drive model geometry toward specified design requirements using the Feasibility study. We then looked at how optimize our model geometry. Before running a feasibility or optimization study, we first explored how to create Datum Analysis Features and User-Defined Analyses. These tools are used to perform calculations and measurements on your model, and then create parameters for those measurements and calculations such as the model’s mass and center of gravity. Next, a Feasibility study could be setup to explore if a specified design requirement could be meet within a range of parameter values. In our specific example we looked at the feasibility of locating a model’s center of gravity on a specific axis by varying the size of a counter-weight. First, we created an analysis feature that measured the current distance from the COG to the Axis.
Then, we could setup a feasibility study to determine if the COG could be moved to the axis by varying the counter-weight dimensions through a specified range of values.
That feasibility study iterated the counter-weight dimensions through that range of values until the center of gravity was on the axis.
However, this solution of counter-weight dimension values was not necessary the only combination of dimensions that would accomplish the goal of having the COG on the axis. From there we ran an optimization study to find the particular dimension values that not only located the COG on the axis, but also yielded the model with the least mass.
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Follow-up Q&A
As usual, there were many excellent questions posed during the webcast. Here are some answers to those question.
Q: Can you drive the model density using the Behavioral Modeling tools?
A: Yes. You may use the MP_DENSITY Parmenter in the Behavioral Modeling tools.
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Q: How do you add columns to the Model Tree to display parameter values?
A: At the top of the Model Tree select Settings > Tree Columns
Then choose the type of column to add (such as Model Params):
Next, select the parameter name and the double arrow:
Choose OK, and the column will be displayed in the Model tree.
Posted by Rand 3D on 04/05/2019 at 10:45 AM in Creo, Webcasts | Permalink
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By Natasha Reaves
We recently hosted a webcast covering the updates to Creo Parametric 4.0. If you missed the webcast, you can view the recording here.
Rand 3D Technical Training Engineer, Natasha Reaves, answered questions that were asked during the webcast, and summarized her responses below. This is part 2 of the Q&A. Should you have any additional questions, please send them to: [email protected]
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Q: Do we have a Weld Symbol Palette yet?
A: I could not find a weld symbol palette
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Q: Are there any changes to the relations, family tables, pro/program?
A: There are no changes to family tables. There are no changes to Pro/Program. There is an enhancement to relations
In the Creo 4.0 Relations dialog box, there is a new Look In option, Weld Solid.
Creo 4.0 Relations dialog box
Creo 3.0 Relations dialog box
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Q: Will the color mapping originally created in WF5 work on Creo4? I opened an assembly created in WF5 in Creo 4 and all models were black
A: Yes. The color mapping originally created in legacy versions will work in Creo 4.0. I tested several of my models, even ones created using ProENGINEER 2000i2 and WF 3.0. All of them opened in Creo 4.0 with the originally assigned colors.
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Q: Are there cheat sheets available from PTC that shows what was versus what is in the UI?
A: I have not found a cheat sheet yet. There have been ones for previous versions of the software. When I become aware of a good one, I will recreate a new post with a link to it
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To learn more about the updates in Creo 4.0, join one of our update classes or contact us at [email protected]:
Posted by Rand 3D on 12/11/2017 at 05:06 PM in Creo, Webcasts | Permalink
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We recently hosted a webcast covering the updates to Creo Parametric 4.0. If you missed the webcast, you can view the recording here.
Rand 3D Technical Training Engineer, Natasha Reaves, answered questions that were asked during the webcast, and summarized her responses below. Should you have any additional questions, please send them to: [email protected]
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The following charts give information about platform support and system requirements for Creo 4.0.
Q: Is there file Compatibility between Creo 4.0 and previous files?
A: Any files that were created in legacy versions of the Creo Parametric (Pro/ENGINEER) software are compatible in Creo 4.0. The model tree will show the legacy model tree listing. And any additional detail added to the file while in Creo 4.0 will list in the modern format. Whether legacy or modern, selection and editing is conducted in the same manner.
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Q: Can Boolean Operations be done in the part or only assembly?
A: The Boolean Operations option is an assembly enhancement. The Merge and Cutout component operations have been combined into the one Boolean Operations option. The tool enables you to select Merge, Cut or Intersect.
In the part environment, the Merge/Inheritance feature has been updated to include Merge, Cut or Intersect settings. This tool will create either an external merge feature or an inheritance feature in the part model.
This tool will create either an external merge feature or an inheritance feature in the part model (no common assembly is required).
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Q: When selecting the sketch references on the fly is it important to select an edge or surface? Or does it matter?
A: It may matter. Your sketched geometry will be more stable if surface references are selected. This will help to build a more robust structure in case editing is necessary later
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Q: Boolean operations - When merging a part object to another part, how does the Model Tree treat the merge feature? Does the Model Tree populate with the merged model features?
A: After the Boolean operation is completed, there is a single merge feature in the tree. The resulting merge feature appears the same as those created in earlier software versions with the old merge and cutout operations.
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Q: Is there a transparency option or button?
A: There is not a transparency display style option for part models. But, there is a transparency display style option when creating a component display style in an assembly model.
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Q: Are there any major difference with the config.pro
A: No, there are no major differences.
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Q: Will all legacy data form previous version of Pro/E come across ok?
A: Yes. All legacy data will appear in Creo 4.0 as it was saved in legacy versions. Whether legacy or modern, selection and editing is conducted in the same manner
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Q: Is there a semi transparency button in Creo 4.0?
A: No.
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Q: What about hardware requirements for Creo 4.0 software?
A: The following charts provide information about platform support and system requirements for Creo 4.0.
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To learn more about the updates in Creo 4.0, join one of our update classes or contact us at [email protected]:
Posted by Rand 3D on 12/11/2017 at 04:30 PM in Creo, Webcasts | Permalink
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Thanks for joining our recent webcast, Updates to Creo Parametric 4.0. If you missed the webcast, you can view the recording here.
Rand 3D instructor, Mike Brucker, answered questions that were asked at the end of the webcast, and summarized his responses below. Should you have any additional questions, please send them to: [email protected]
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Q: Any way to turn off all pop ups when you are doing things?
A: I don’t believe you can disable the yellow notification windows globally. However, some, but not all, of those notification windows will have a checkbox at the bottom to not show that window in the future.
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Q: Can you have the automatic simplified reps and custom created reps active at the same time? That is, run generally on automatic, but also have maybe a "No fasteners" defined rep.
A: You can only have one Simplified Rep active at a time. However, each component within any Simplified Rep can be set to Automatic or Exclude.
In this example, we set the top-level assembly to the Automatic representation, selected all the hardware from the tree, and set the hardware to the Exclude representation.
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Q: When a layer is hidden and it hides the features, does that actually hide the feature in the model tree as if you had hidden the feature itself? Hiding in the model tree is no longer independent from the layer functions
A: The hiding of individual items and the hiding of Layers are still two independent functions. The only change to Creo 4.0 is that the Model Tree will show the hidden items grayed-out regardless if they were hidden individually or belong to a hidden Layer.
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Q: Are there any rectangular tubing creation tools? I'm asking this because we usually create a 3D model of tubes to be imported for tube laser programming.
A: Yes, Creo 4.0 does have a Piping application for creating pipes, tubes, and hoses of any shape.
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Q: Can you turn off the Auto Ref. in sketcher mode?
A: Yes, there’s a configuration option to disable the new automatic selection of sketcher references from model geometry in Creo 4.0. File>Options>Configuration Editor. Set “sketcher_snap_model_geometry” to No.
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Q: Showing my age here, but can we have the classic ProE blue graphic back as a selectable option for the backgrounds?
A: The old blue background color is not one of the predefined color schemes in Creo4.0, but you can still manually set the background to any color you want. File>Option>System Colors>Graphics>Background.
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Q: Is there anything different with printing drawings?
A: Yes, Creo 4.0 has several enhancements to drawings. Many of these are related to creating and displaying Geometric Tolerances and Datums. Here are a couple examples:
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To learn more about the updates in Creo 4.0, check out our latest Creo Parametric 4.0 class: Creo Parametric 4.0: Core Update from Creo Parametric 3.0
Posted by Rand 3D on 06/15/2017 at 04:52 PM in Creo, Webcasts | Permalink
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Can't join Dassault Systèmes in Santa Clara at Levi's Stadium for the #3DEXPERIENCE FORUM? Registration is now open for the Live Stream!
Register and View it with Rand 3D!
November 10, 2016 | 10:00AM-12:30PM PST.
Posted by Rand 3D on 11/09/2016 at 03:20 PM in Industry News, Webcasts | Permalink
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3D solid modeling programs have always held great promise in the possibility of reusing the models in downstream deliverables such as:
Somehow that promise has never been realized. There are a number of reasons for it, but two major reasons are software capabilities and ease of use. Although all the major CAD systems have tools for capturing 2D images and creating animations it is not the focus of the software. They are engineering design tools first and foremost and always will be. Complexity also overwhelms the casual user.
Recently this has begun to change with a new generation of programs focus solely on the downstream possibilities. One of these programs from Dassault Systèmes is CATIA Composer. CATIA Composer lets you quickly and easily repurpose your 3D data. If you think you could benefit by this, we recently ran a webcast looking at CATIA Composer and explored some of its possibilities. Take a look:
Posted by Rand 3D on 06/24/2016 at 02:44 PM in CATIA, Webcasts | Permalink
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