Another Creo Newb looking for advice

[TheNinjaStyle]

I'm new to Creo and using the 'Foundation Adv" license. I need some recommendations for a book or two to help get me started. I'm one of those people that are used to SW and Inventor, heck I find modeling in Acad easier right now

It seems like Creo has a huge amount of options and youtube and PTC videos haven't done me much good. With all the available options it has to be robust so there must be potential; and I hate to be the speed bump in the way of productivity during the design process.

I have a handle on the modeling basics, but any recommendations for books should definitely be for a beginner.

One more quick question, I can't find the option to break all of the references in a part that was designed in the context of an assembly, like break adaptivity or associativity, the reference viewer does not help me.

How can I break these references without redefining or losing information. Like, for example, if I had created Part C using the surface of Part A as a sketch plane and extruded it to the surface of Part B, and projecting Part A's sides as my sketch... how can I make Part C no longer dependent on the other parts for it's geometry to be created.

Thanks for any advice

 

[design-engine]

Ive found people with 20 thousand hours can model stuff but they don't really know basics like selection tools.... they turn off the selection tools from smart etc. You can learn so much from having someone that knows the tool help you... sit next to you. There is so much to learn. Lucky for you many of the icons are similar to SW

Break references. Why would you want to do that? You edit definition on the part while in Assembly mode. There you can right click the references and remove them one at a time. There is no global reverence delete function.

 

[dgs]

SW and Creo are similar on the surface but quite different in fundamentals.

SW seems to be built to reward speed and you're able to create and recreate things fast. Things fail, you redo them because that's easy and fast.

Creo seems to be built to reward careful reference selection and deliberate modeling. Take your time, pick the reference that matters and you're model will be very stable. Things shouldn't fail as often (that's my experience) and when they do, there are many tools to find out what it was and how to fix it.

In the case of your assembly, there is no simple way to break those references without going back into the assy and redoing it to pick new references. The assumption is that you built it that way because that was important to your design intent so breaking them has to be done in the same way that they were created.

People who get this, get Creo and love it.

If you try to drive Creo quick and dirty like you can SW, you'll be frustrated. Conversely, when I try to drive SW like Creo with deliberate reference selection I'm frustrated because it just isn't built to respect that. I prefer Creo's focus, but there's a place for each.

 

[TheNinjaStyle]

Unfortunately there is noone here to show me the ropes so I will have to learn as I go. I didn't want to go bottom up for design but it looks like it will be the best way to start. I appreciate the help.

 

[Jacoolo]

as Bart said - directly in appropriate parts by redefinition of features.

there is no global/general tool to remove external references form parts(I wish to have such)

you can also open depended parts in session separetly(no final assy avaialble in session) and redefine each feature which share external references. Pro/E should then ask you to keep them(references) ot not. Neverthelsess, there is some effort involved, because some feature, like sketches will require to indicate new references.

 

[TheNinjaStyle]

I guess I will have to be a little less lazy with my modeling What I am doing now is not as much top down; I still model all the parts in the assembly but I am conscientious not to reference my other parts and then assemble them. I prefer not to have to go back through and redefine since I am still a novice and it is much more time consuming for me and most of the time I have this look ->

On the plus side I feel like I am thinking a little more but at times I am feeling less productive. I will try creating some parts with references and redefining them when they are opened individually. Maybe it will speed me up a little. Thanks

 

[Jacoolo]

if you picked up TDD as a way to go, you should be then no suprised about bunch of external refs spinned all around

maybe you are not aware of, but there is an option to push pro/E to allow referencing only to skeletons and layout models. more, you can push pro/e to allow referencinfg only to Publish geoemtry features.

then there is no random edge as reference picked up by accident in the sketcher - consider this.

 

[dgs]

Solidworks is much more forgiving of lazy or sloppy technique, Creo tends to punish it. However, the reverse is also true, careful modeling can make Creo sing, where in SW it matters less.

TDD is Creo is extremely powerful, when done carefully. Look into skeleton driven TDD and copy geom & publish geom features. Very robust and powerful stuff.

 

[michaelpaul]

Unfortunately there is noone here to show me the ropes so I will have to learn as I go. I didn't want to go bottom up for design but it looks like it will be the best way to start. I appreciate the help.

I understand what you are asking to do but as everybody has mentioned, there's no easy way to just break your references. without anything to define the feature they would simply fail as the software wouldn't know what to do with them.

what you probably should/could have done from the start (and I don't blame you since it's not the obvious solution when you're learning) is to create a skeleton model with your master model constraints. then you can publish that geometry from the skeleton into individual parts and reference the planes, sketches, surfaces, etc in a part. that way, the only exsternal references are to published geometry in a single model not to multiple different parts in an assembly.

 

[PROMOUSER]

If you must....

1. Set your working directory and open your top top level assembly.

2. Take one part at a time.

3. Pull it out and put it in a folder other than your working directory and rename it to something else.

4. Rename your top level assembly.

5. Put your renamed part that was quarantined back into the working directory.

6. Open it.

7. When it begins to fail, just walk it down.

When a feature fails it might be as simple as opening the sketch. Open the reference list. Delete all references. Select a coordinate system for a reference. Don't touch anything else. Close the feature, and go to the next one.

When you're done you will have a part that is not referenced anywhere.

8. Save your file.

9. Rename your assembly and parts as needed.

10. Beware any drawings that reference your parts will look for those by name so pay attention to what you are doing.

Parts should never reference other parts with the exception of fasteners and other items that are easy to correct and are self-explanatory.

Bottom up modeling is the curse of the true professional, and the sign of a rank amateur. Unfortunately, it is how most of us learn to model assemblies. It is an obsolete concept in this day and age.

Top down is the only way to go.

You need the AAX (Advanced Assembly Extension) to really take advantage of top down design.

I would recommend taking classes at Design-Engine in Chicago. They''ll teach you how to use the tool in a week.

Here is a quick tutorial on the concept of top down design.

TDD Pocket Demo, Free Pro/E Wildfire Video Tutorial, Consumer Product Design/Development, E-Cognition Inc

Remember: It's how fast you can change a design 20 times that matters more than how fast you can model your initial concept.

Professionals use professional tools. NX, CATIA or Creo. Wizard based mid-range modelers are good if you are drawing circles and rectangles.

Creo rules.

There - my first post to MCAD CENTRAL. Hope it helps.

 

[headrush]

My advice is to change software. And remember that the execution of the concept of parametric modelling is flawed (except between a drawing and the part it references). I do not reference anything in my designs. Each part is completely independent. In the long run I believe it's the best approach. References will eventually bite you in the rear. And it will draw blood.

Remember the KISS philosophy.

 

[PROMOUSER]

I couldn't agree more.

Yes, yes & yes.

The KISS principle is what it's all about.

You don't have to reference anything other than a coordinate system in Creo, so in essence you don't have to have any references or relationships. I prefer to leave my features "loose" like that too - rather than reference existing geometry.

That's the whole point of true top-down design. You only tie geometry that is shared between parts (think conformal battery door on the back of a surfaced device) to datum geometry.

Referencing other geometry or other parts is not top-down design. That is painting oneself into a corner. I would rather have no references.

See the attached image of a "perfume bottle". There are no dimensions driving this model. There are a few control curves that can be pushed and pulled to morph the geometry.

Switch programs at your own peril. Creo is awesome.

 

[dgs]

... And remember that the execution of the concept of parametric modelling is flawed (except between a drawing and the part it references) ...

I absolutely disagree. I extensively use top down design and skeleton modeling and lots of parametric references to the skeleton and feature to feature within my parts. It has saved my countless hundreds hours of rework. Parametric modeling is profoundly useful and excellent at capturing the design intent of the entire product and maintaining it through changes.

Perhaps you meant the execution in Creo is flawed and I'd have to disagree again. I've only used Creo/Proe & Solidworks, but I'd take Creo any day due to its robust reference management capabilities. SW simply doesn't respect my reference choices as much nor does it give me the tools to manage them, and therefore my designs.

 

[PROMOUSER]

I'm all about TOP DOWN design if you are using skeletons, and doing it the correct way.

Some people think that building models BOTTOM UP and referencing each other is TOP DOWN, and they are wrong, and then they argue against TOP DOWN design. Evidently they are not teaching the method properly in our schools.

All I'm saying is that I would rather have no parametric references than something that has been designed BOTTOM UP.

Creo is the best. By far.