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"exclude from bill of materials" / "envelope" feature

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Re: "exclude from bill of materials" / "envelope" feature

You can create a new Skeleton Model by using the Create function in an assembly and choosing "Skeleton Model" as a type. You can also convert any existing part to a Skeleton Model. To do that, you need to put it at the very top of the model tree (Before any planes or csys. You might have to do it in two steps, moving the part almost to the top, then moving the first feature below it). After that, you can use the Replace command, choose By Copy, and check the Copy as skeleton checkbox.

It sounds like you're trying to do someting in Creo the exact way it works in Solidworks, though. That's a recipe for disappointment. Creo is not SW, and trying to use it the same way will just lead you to use cumbersome solutions and unnecessary clicking. What you're trying to do might be easier to do using Copy Geometry or Shrinkwrap, for example.

In the end, if you have to work in Creo, complaining about how it's not SW will get you nowhere. Perhaps it's not as good, but in the end it's what you have to work with, so you're probably best served by trying to learn how to work best in Creo.

Re: "exclude from bill of materials" / "envelope" feature

Its funny because we use a 3D cad software but we cant do 3D sketchs…. (80s technology…)

Datum points are not 3d sketch at all, are time consuming, limitated, and you must use a lot imagination to create things with that. 2020 year and we still thinking in a 2D way….

The mirror feature (new one also) its a **bleep**. Sometimes I dont want to make a group just to make a mirror. Why I cand just select 2, 3, or 20 parts and do the mirror? make no sense. 

Also, there is nor posible to select the "orientation" of the mirror when you use the "reuse" option, I mean, sometimes you do the mirror operation and the part its flopped on the wrong position. SolidWorks gives the option of 4 "positions" when you do the mirror, so you can orient it in the right way. This must be done manually on PTC and you break the link between position of the main part. If you edit the position of the main part, you must edit the mirror part also. Time lost...

Transparent components doesnt exist on Creo, I mean, if you turn to transparent, all assembly makes transparent. On SW you just select the part (or sub assembly) and just that part turn to transparent. 

Groups is nor the same than folders and sub folders on the tree.

Assembly components in any order: On Creo, you must pay lot of attention on the assembly to the order of the components, because the mates are **bleep**. Also if I delete one "top" component, the software isnt enought "smart" to break the mates to the other components and not delete it also….

Auto repair at the end requires a manual work. Time lost. 

Copy paste on sketch doenst work, if you want to reuse an existing sketch you must create it into the "palete". On SW its just copy paste.

 

I dont think Creo its more powerful than SW, as I see its just more "dummy" soft with old way of work methods. Not customer oriented, not productivity oriented. We are in the 4.0 era and we still working like 20-30 years ago...

 

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Re: "exclude from bill of materials" / "envelope" feature

Im not necessary want to do it in the same way of SW, but yes to get the same result. That s why I asked how others work with assemblies but any one seems to be working like this.

I will try the process you said, but seems to be too complex (time consuming).

I will check copy geometry and Shrinkwrap (I dont know anything about that).

According your experience, if you are working with a complex / multi options machine project, how you position the parts refferenced to main machine assembly?

As I know, the most used solution on PTC is place it on the main assembly, then make it fix. It works but if you change anything on the main assembly then the "fix" sub assemblies remain outdated… (more manual work to re update it)

Another issue on Creo is the (bad) support...

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Re: "exclude from bill of materials" / "envelope" feature

Again, FWIW:
Of course you can turn individual components transparent in Creo. Select the component, then do Model display -> Component Display Style -> Transparent. Again, I like to put it on the popup menu, making it very quick to turn any part transparent.
And yes, you can delete any component anywhere in the tree and keep all the other components, even if they have references on them. Click the "Options" button in the delete popup box and set the components to "Suspend". Then use things like the Edit References command to reroute the references, a simple Fix mapkey to remove the constraints, or better yet, use the Replace References to reroute all references pointing to the component or feature you're about to delete before you delete it. Reference handling is one of those things I've heard a lot of Creo users switching to SW complaining about ...
And copy/paste within and between sketches works without a hitch in Creo. Select the sketch geometry, copy it, then paste it in another sketch. Tip! Do the same with features and geometry. You can do a lot of great things in Creo by copy-pasting surfaces, modifying them and then solidifying them again, and the paste special functionality can do a lot of cool stuff, too.
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Re: "exclude from bill of materials" / "envelope" feature

For complex projects, using Skeleton parts and Copy Geometry to do Top-Down design is usually beneficial. You can put geometry in the Skeleton that you use to then copy into your parts to build them, meaning a change to the skeleton will update both parts and placement. For complex project, one skeleton per assembly level, copying geometry down into the structure can be really powerful if well implemented. Add Notebook functionality to this, allowing you to push global parameters into local parts and subassemblies. Your parts can then simply be placed in Default, and will update their placement when the Skeleton updates. Research Top-down Design. There's a pretty good book on Amazon explaining the basics.
I've also seen quite complex machines using just the regular old constraints and it works fine. I'm not a big fan of relying too much on the fix constraint, myself. You gain stability but lose flexibility. And remember, sometimes you WANT the model to crash. It's a sign that something is wrong. When you've changed the hole pattern your bracket is attached to without updating the bracket, that constraint should fail to tell you that things don't fit anymore. Depends on what you need to do. Simp reps are often used to control variants/options, and automatic rep to avoid long loading times of large assemblies. If you have a lot of options in your machine, that's what the Options Modeler module is for, though I think that one could stand to gain some more development attention. I think it tends to come in the same package as the Design Exploration module, though, which is really neat.
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