Learning creo from SW, very basic questions 1

[VanW]

I'm needing to learn creo and could use some help. 10 yrs of experience in multiple other programs NX, SW, Fusion. Thanks in advance for the help.

The parameters have me slightly baffled. It is greyed out when you are in a sketch. Yet you can go into relations and make a parameter, weird.

I guess you have two choices...
1) you make your parameters prior to the sketch which I'm not a fan of it I'm designing a new part or product. I may want to enter a dimension in and see how it works then make it a parameter later.
2) In the sketch you click the relations icon and make a parameter, then you must exit out of the relations to apply it to a line length.

I think in all the CAD programs I've used when you start typing in a parameter name in the dimension field next to a line it populates with all the names you began the letters with. I don't see this happening in Creo. If I have bottom_width and top_width as parameters I always just type in width and both populate on the dropdown. Without this I see I might have to go into relations to remember the parameter name.

I'm I reading the program right or is there an easier way, specially to get the auto populate dropdown of names if you have a lengthy list of parameters?


If I sketch two rectangles in one sketch, do you have the ability to only extrude one of the rectangles? I'm also curious if you can extrude a single leg of a rectangle as a sheet body. In solidworks for instance you have to project(convert entities) the single leg into a new sketch in order to extrude one line from a previous sketch. From my initial test drive, it appears you can't single out a rectangle for solid extrude nor can you single out a leg for a surface extrude. Just trying to confirm what I'm seeing on how flexible creo is with extruding single entities from an intricate base sketch.

If I have two rectangles extruded from two differing sketches, how do I hide one of the solid bodies?

How do you know if a sketch is fully constrained?

Thanks for help, I've got a few more questions, but this is plenty for now.

 

[3DDave]

The short answer - that's how it works.

Whatever you want to represent I expect Creo can do it. However it won't match the workflow of other software, and expecting that is unrealistic.

Long ago a major corp wanted to find the best word processor software and gave half the secretaries access to one and the other half access to the other. They let them use the software for enough time to get a good feel for it, then then had the two groups switch. This way, they thought, the secretaries would have experience in both and see which was better. All the secretaries felt the first one was better than the second one, regardless of which group they were in.

People get used to things and dislike change.

Instead of asking how Creo isn't like other software, identify the results that are important and look at workflows that produce them.

All non-reference dimensions are parameters. You can just change the name.

https://community.ptc.com/t5/3D-Part-Assembly-Design/How-to-rename-dimensions/td-p/320865

You can create a giant complicated** datum feature sketch and then use-edge to create individual features rather then the "sketch a bunch in a solid feature sketch, but don't use all of the solid feature sketch geometry to create solid features." Creo tends to try to make relationships clear by not having multiple levels of indirection as to what the controls are. Since there is that separation later users don't have to wonder why only some of a sketch was used; they can see the independent reference sketch and then see the features that are separately created from it.

If the parameters don't drop down, they don't drop down. I don't recall ever needing a click-to-pick list. I know some software editors use it like those inflatable guides in bowling alleys - to keep programmers from accidentally misspelling a variable name that, in turn, leads to a compiler error [worse, in some languages, the language interpreter automatically creates a new variable - Excel VBA does this unless the "Option Explicit" command is used] but, since dimensions are already parameters, then it would produce a list possibly thousands of entries long.

In the case of separate solid features of a single part, one can create a simplified representation that does not include the undesired features, suppress the undesired feature, or create a family table for which the undesired feature is not included in an instance. It might be that the better answer is to create an assembly of separate parts - in real life components rarely have floating unconnected items.

**The general advice is to avoid complicated sketches. It's not that Creo cannot handle them or that they are unreliable, but that users aren't particularly careful in creating them and few are attentive enough to correctly modify them. I've experience users who would delete the sketch entirely and re-do it rather than make a simple modification, destroying so much work that is based on it. So, make sketches a toddler can handle and avoid that problem.

 

[VanW]

3DDave,

Thanks for the detailed reply. I learned on NX and when I ended up in SW it was a wake up call. NX is just do what you want, how you want imho. I'd have to do some complicated surfacing so I just dove into the project and then eventually when I saw the end coming I would clean things up. I'm not trying to make complicated sketches, but it is damn nice to click one line from a master sketch and just sweep or extrude it as a surface without having to create another sketch and project the single entity onto your new sketch.

I removed weak dimensions as I don't want dimensions tossed in my face that are draggable. Then I auto-locked entered dimensions(should be default imho). Those little changes really took much more time to learn than I'd like to admit. The whole weak, strong, lock is a bit much for me, lol.

So my final question now is how in the hell do you know if the sketch is fully constrained. I don't see a notification or color change anywhere that lets you know. 95% of the time I know when I'm fully constrained, but it's nice to have a verification?

edit....btw not to discount your opinion on the lack of need for the dropdown, but it is damn nice to be able to type in C and get all Chord values I've created, or just scroll down to global variables and get everything at a click. I'm not pumping sw here, I'm just saying the auto-populate variable/parametere/equation whatever a software calls it is a damn nice feature.

TY

 

[3DDave]

All Creo sketches are always fully constrained. If you don't supply enough strong dimensions Creo will add enough weak ones. You can toggle any dimensions to get the result you want or apply others and Creo will remove redundant weak ones.

I recall from other SW -> Creo converts that SW didn't enforce full constraints, causing new Creo users much heartburn. Maybe SW changed that, but it seems like it was that way for a decade or more. Those in favor of non-constraints said they liked not having to do constraints until later rather than having to figure out what they wanted to control vs. what geometry they wanted to have up front.

You can make locking the default.

http://support.ptc.com/help/creo/cr...her/About_Locked_and_Unlocked_Dimensions.html

 

[VanW]

Dave,

Damn you're fast...I need to think about what you said about creo being fully constrained. I'm not so sure I agree that a point that can be dragged around by a user click is constrained. That's what blew my mind was a strong dimension 'entered by user' could be manually moved so I immediately auto-locked that feature.

I don't know what you mean about SW enforcing fully constraints...you are at liberty to completely underdefine your work, but that's at your own peril. Here is SW warning at the bottom that you are underdefined.

 

[VanW]

Dave,

I think the constrained issue is a grey area and is perspective. I'd argue hard against the creo approach, here is why...So a fully strong sketch in creo is deemed fully constrained. So is a fully weak sketch. If I go into another software and fully dimension a sketch then delete all sketches, what do I then have? I have a 100% desired sketch to spec, yet completely unstable and more importantly unreliable. I'm no expert, but when you can't move points on a sketch manually, I deem it 98% constrained. The other 2% confuses me, don't ask.

tY for the replies. I'm off to learn the surfacing tools in creo, they bent my brain backwards last night.

 

[3DDave]

Yeah - that cannot happen in Creo. There are no underdefined sketches.

Edit:

Constraint as in - the geometry solver has all the equations required to produce a single result. Not - cannot be modified by further user interaction.

 

[Korichnevijgigant]

Sketches are fully constrained because of the absolute references, when you set up a sketch you have to pick 2 absolute references (think X and Y) and everything goes to these 2, in later Creo versions this is done pretty automatically, in older WildFire days, you had to pick the 2 surfaaces, datums or whatever that represented your absolute references

You can still drag points around, up until you "lock" dimensions, then you cant drag

but weak and strong dimensions can still get drug around and modified

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[Korichnevijgigant]

Also I think you will be very happy with Creo once you get over the learning curve, I cut my teeth on Wildfire/Creo and then had to go use Solidworks and NX for a number of years, NX wasnt bad, but man I do not miss the strange instability and assembly mates and overall performance of SW, we used to call it SortaWorks

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[bartbrejcha]

I've pushed solidworks very hard over the years and have found it to be a bit on the saladworks side of the fence with parent child relationships not holding as they should *compared to Creo But overall it's not so bad.

Bart Brejcha
Design-engine

Bart brejcha training consultant

http://www.designengine.com