New WF4 User, Catia V5, SolidWorks, I-Deas background

[weroberts]

New Pro-E user.
A Few Quick questions. In Catia and Solidworks when you define a sketch and actually place dimensions on lines and arcs you can grab and move around the other geometry in relation to how you have these dimensioned. The dimensions do not change.
This does not seem to be so with Pro-E. If you draw a square and then dimension two sides then grab a corner it ignores what ever dimensions you put there.
This really bugs me and works different then any CAD package I've seen. Is there a way to fix this behavior?
Or is this just how it does it?
In drafting is there really no way to show a centerline for a radius?

Going from I-Deas to SolidWorks and Catia was way easier then Pro-E

 

[kirrer]

YES! I had the same issue when I started using Pro/E (native Catia V5 learner here). The difference is in Catia, when constraining a dimension it becomes 'locked' until you edit it again. This functionality is possible in Pro/E by 'locking' a specific dimension (right mouse > Lock). Of course, that would be time consuming for every dimension, so I enabled the option 'sketcher_lock_modified_dims'; now, any time I modify a dimension I create, it's automatically locked, which is enough for me. There's also 'sketcher_dimension_autolock' which may be also desired.

I can't answer the drafting question, though.

 

[jvian]

To increase the productivity of locking dimensions without the system automatically locking all modified dimensions, you can first create your dimensioning scheme then cntrl+click all other dimensions which you want to tie down and lock them all at once. This became our preferred path since the locked dimensions can get in the way of dynamic edits in Creo 1.0 which we use frequently. Locking the dimensions will give you the functionality you are after however strong dimensions will not. They will change in value just not intent.

Centerlines for radii in drawings are shown by using "show model annotations" then selecting the "datums" option and picking which ones you want. This may be very different depending on the version of pro/e (or creo) you are using.

Some free tutorials are available at

http://learningexchange.ptc.com/

however most are for Creo and newer versions of Creo Elements/Pro. Also check out the knowledge base at ptc.com. Can be hard to find what you want but there is a lot of information there too.

Hope that helps,

-J-

 

[jmadd]

Regarding the drafting question:

Depending on how the radius was created, it may or may not have an axis that can be displayed. If you don't find an axis to show using the "Show/Erase" function, you can go to the model and define a datum axis through the radius. Then you should be able to show it in the drawing.

John

 

[mjcole]

1. In Catia and Solidworks when you define a sketch and actually place dimensions on lines and arcs you can grab and move around the other geometry in relation to how you have these dimensioned. The dimensions do not change.
2. In drafting is there really no way to show a centerline for a radius?

ANSWER 1:
This statement is not true at least as far as SolidWorks is concerned. SolidWorks has an option in Tools > Sketch Settings to Override Dimensions on Drag Move and if it's checked on, your defined dims will be modified as you move geometry.

For SolidWorks it's all or none whereas for ProE you can chose which dimensions you want to allow or disallow to be modified with Lock Dims options.
(The only way to lock a dim as such in SolidWorks is to write an equation for it.)... wait Even if equation is entered dims still get modified when dragging geometry if override is enabled
Check that you can only allow modification of selected dims by turning the modify dim on drag/move option off and making the dim you want to change driven.

These options can be set by config or from Sketcher Options dialog
Sketch > Options on [Miscellaneous] tab
[√]Lock Modified Dims is equivalent to sketcher_lock_modified_dims yes config
[√]Lock User Defined Dimensions is equivalent to Sketcher_dimension_autolock Yes
https://lh6.googleusercontent.com/-xD4EBaWBDow/Tu10lYj7pfI/AAAAAAAADY8/YdtVfmhmVqY/s400/proe_sketch-Options_dialog.PNG"

[uANSWER 2:[/u] <<<<<<<<<<<<<<<<<
ANSWER 2:
"WHY is TGML not working tonight??????????"
By radius do you mean Fillet or Arced geometry? I'm assuming arced geometry but Axes can be shown on fillets in SolidWorks see image.

There is an option for this but I'd use it on an as needed basis. If you need them turn the config option on before extruding and shut it off if it will make excess or duplicate axes.
The option is show_axes_for_extruded_arcs yes/no* I believe it's no by default which explains the behavior you are not seeing.
To get axes for fillets you'll have to make a datum axes through them manually.

ProE's sketcher allows way more intuitive constraining and will allow you to lock multiple constraints by Shift Right Click to lock a highlighted L1 or H or V or disabling with right click. In Wildfire WF5 Right click toggles constraints active or inactive on each click. You could sketch a hexagon and lock equal length and parallel constraints all to together SolidWorks currently doesn't support equal length relations except by Linked Dimensions

Michael

 

[weroberts]

Thanks for the settings. I like them already. Forgot to mention I'm running WF4.