the best way to assemble in CREO2

[bp]

Since a few day I have been working with CREO2 coming from WF5.

There are 3 things that bother me:

1. When I start mating, it usually starts with "automatic", but 99% of time I want the coincident constraint which is often not automatically recognised. Is there an option to modify this?

2. I dont use the 3d dragger, can I get rid of this forever?

3. When assembling, I usually go to a window with a (new) part,

then put the name of this part to be assembled in memory (clipboard) by copying the part's name from the message log after I press "save"

and then activate the assembly window and paste the "to-be-assembled part" name in the "assemble" dialog box in the activated assembly window.

I've made a mapkey which copies the name of any activated file to save time.

I do it this way because CREO doesnt support drag-and-drop of parts in an assembly from other windows and I usually work with large assemblies with names that consists of only digits.

My question is: how do you guys assemble? Is there a better way?

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[James62]

hi,

My answer to all 3 is: mapkey, mapkey, mapkey.

There is an icon in dashboard to turn off 3D dragger, but no config.pro option to turn it off permanently. So you can set up a mapkey and press it everytime when the dragger bothers you.

Same with the coincident constrait. I'm doing this using a mapkey.

For the third point I've got a question. I always thought that ctrl+c (copy to clipboard) can't be used inside a mapkey. How did you overcome that one?

[bp]

Thanks for your answers!

I overcome the "copy name" problem by creating a mapkey which does the following:

first create a log-file which contains the name of the current part in the working directory.

Then a batch file with DOS script copies this name to memory and then the log-file is deleted.

I also use this method to open drawing files from asm/parts with the same name automatically

and also to quickly add part-instances to a drawing file.

Im sure you can do this even more efficient with Pro/Toolkit but I'm not familiar with that nor do I understand why PTC does not just program these mapkeys themselves.

If you're interested I can post the code for the "copy file name" mapkey.

[James62]

You're welcome.

I would like to be able to do ctrl+c, ctrl+v, and ctrl+a with mapkeys. It would really help me alot, but I don't think I'll understand the scripting file.

Oh, well... *sigh*... Please share, and in case you consider this as your own intellectual property, just poke me via private message with it.

I am totally interested.

Thanks in advance.

~Jakub

[TomD.inPDX]

I see a view Ideas in your post. I suppose the only other enhancement that may be useful is the component interface option.

Assembling has never been fun in Pro|E. I like the idea of remembering the last series of mating conditions used; having the part pop up on the screen where you are zoomed rather than 0,0,0; allowing several of the same parts to be inserted at the same time to sort them out after the dropping them... and mixing them up a bit so they don't all lay on top of each other... but I do like that it remembers the last component placed. I also like the iconography (preview) of the part files. Not always clear but a feature I do find useful.

Isn't there a way to automatically assembly a lot of parts through a script of some sort? I'd love to just build a BOM and let it drop a bucket full of parts in the assembly to be mated after the fact.

[bp]

I've placed a tutorial online.

check out http://communities.ptc.com/docs/DOC-3535

[James62]

Thank you.

[obienate]

In response to issue #1, I found a method that helps the "automatic" constraint so it doesn't pick dumb options that don't make sense. Add these two options to your config.pro:

comp_angle_offset_eps 91

comp_normal_offset_eps -1

This will generally use "Coincident" the way most of us want. Why did it always default to "Normal" and who would ever assembly something that way?

Has anyone found a solution to to issue #2? It would be really easy to have this as a config option...

[StephenW]

No, officially you can't disable the 3d dragger for more than the current session.

I submitted a product idea to add an option to give the user the ability to have it turned off by default but the user can turn it on using the dragger icon if they want to use it. I consider it synonymous with the option to turn off the spin center.

http://communities.ptc.com/ideas/3996#

I give up, just copy and paste the line above, I can't get the link to work.

[TomD.inPDX]

Correct link: 3D dragger in assembly - allow a defualt to be set in the Config.pro