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Query Select in Creo?

Marble

Query Select in Creo?

Ok this has been bugging me for some time. I was doing a lot of assembly this morning and it's just a real pain in the neck. (Or possibly lower down than that.)

In ProE, it was easy to query select the back side surface. In Creo, I can't figure out how to do it. I have to keep rotating the model around to have the surface face me before I can pick it.

Also a lot of the time the damn drag do-wicky is in the way when trying to select a surface on the component your placing.

So how to you query select?
How do you turn off the stupid drag do-wicky? (3D-Dragger)

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550


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19 REPLIES 19

Query Select in Creo?

Turn off the drag do-wicky here.
[cid:image001.png@01CF3A1E.4D1BC850]


If you have the pre-selection hightlight turned on, query select is as simple as right-clicking through the surfaces (and edges and vertices). You can also right click and hold and get the "pick from list" box which used to be the query select bin.





Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

Oops, it was supposed to have an arrow pointing at the icon to turn off the assembly thing-ama-bob.

[cid:image002.png@01CF3C2A.29DC7340]


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

Good question. Not that I know of. The good thing is that once you turn it off in a session of Creo, it stays off for that whole session.

Anyone know if there is a config option to turn it off to start with? It’s usually in the way of selecting a plane or axis I want to use as a constraint so it almost immediately gets turned off in every session anyway.


?

Steve,

Do you know of a config setting to turn this useless thing off rather than having to do it with each component?

Thanks,




Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

RE: Query Select in Creo?

Using CS48699 for information about the 3D Dragger I tried this as a solution. That CS says that the 3D Dragger remembers the last state (show or hide) within that assembly. It appears to be working.


Open your start .ASM file. The one stored in your config location START_MODEL_DIR.


Assmble a part. (I used a random file already in my workspace. It may be a better idea to use the start .PRT file.)


Turn off the 3D Dragger.


Complete the assembly of that part (I left it unconstrained).


Delete the part from the model tree.


Save and Check In the start .ASM file.


Now when you start a new assembly using that as your template, the 3D Dragger should be turned off when you assembly any part or sub-assembly.




In Reply to

Query Select in Creo?

That didn't seem to work for me, at least on my set up. Creo 2 M060.

I created a new assembly and assembled a part during which I turned off the dragger. I tested it in the same session and the dragger continued to be turned off for the next component. Then I re-started CREO and opened up that assembly and assembled another part. The dragger was back on.

I believe the last "remembered state" is per CREO session and not per assembly.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

I just submitted a product idea on the PTC Community to give an option to turn off the dragger. Feel free to vote on it.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

I see multiple problems with this solution.

First, we run multiple versions of Proe / Creo and have active work in WF4 AND Creo2. We would not want to lock our start parts into Creo2 nor maintain multiple sets of start parts.

Second, this sets globally what is really a user preference. I may hate the 3D Dragger, but other users may like it. Setting it to be off for all violates one of the tenets of my philosophy as an admin - don't lock down globally what is simply user preference and does not affect model quality. I want to give my users all the freedom to work as they prefer that I can.

--
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Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

RE: Query Select in Creo?

I may be the only one that thinks the Drag Orb is actually a very good tool on this thread, but all my engineers love it as well. It gives you instant feedback on not only the degrees of freedom the component has, but which ones are free. This aids us in knowing very quickly what constraints are in place and which ones are not.


We also use it to drag the component in place or in the general location that we want to place it but at the same time, you can drag the component away from any surfaces you may want to select for placement.


One of the reasons our assembly time has gone down drastactly, is due to the Drag Orb.


I wonder if others out there see the good in this feature?. Maybe if you try to work with it, instead of around it, you may find that it has good possibilities.


Query Select in Creo?

I’m on board with the Drag orb. That has been a great feature in Animation/ Modeling software for years. Makes the process more like real modeling and less like programming. Everyone here loves it as well.

Query Select in Creo?

It comes in handy but when I know exactly what how I want to constrain a bolt in a hole and I can't select the surfaces until I zoom in or out because the dragger is in the way, that's when I get frustrated with it.

I do use it on occasion but 9 out of 10 times when I am assembling a part (or sub-assy), I know exactly how it's constrained and what I need to do to get it fully placed.

I would just like it not to be there unless I tell it I want it, like datums and spin center. I'm fine with the default setting of the dragger to be turned on, I just want a customizable option to turn it off and for it to stay off until I need it.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

Ok, call me the luddite of the group, but I like the old two window method the best.

More often than not, I'm assembling small parts into a large assembly. I can have the small window zoomed up at one scale and the larger window at another scale.

One thing the kind of irritates me now it that the process wants you to pick a reference in the assembly before picking the part reference. That's backwards from how I've been working since 1989.

And actually there are times I miss the insert option.

David Haigh

RE: Query Select in Creo?

At the end of the day, we all work a little different and have different scenarios. I think it only makes sense for it to be an option. One group would use it often and turn if off when they don't need it and another gourp would rarely use it and turn it on when they do need it.


Bottom line is that it should be a config.pro option and we should all push for that.



In Reply to

RE: Query Select in Creo?

David,



On my end, I can pick a component reference first or assembly reference first. My choice. Not sure why yours is working differently.

In Reply to David Haigh:


Ok, call me the luddite of the group, but I like the old two window method the best.

More often than not, I'm assembling small parts into a large assembly. I can have the small window zoomed up at one scale and the larger window at another scale.

One thing the kind of irritates me now it that the process wants you to pick a reference in the assembly before picking the part reference. That's backwards from how I've been working since 1989.

And actually there are times I miss the insert option.

David Haigh

Query Select in Creo?

Also, the pre-orb method of holding Ctrl+Alt with either middle mouse button or right mouse button still allows one to dynamically rotate or move the component during placement. (MMB is dynamic spin, RMB is move.) Constraints will restrict this movement, acting as an indicator for what else needs to be constrained, also just like the orb does.

Query Select in Creo?

I agree. I can pick either the assembly or the component reference. I justed tested it in the separate window alone, when both the separate window and in the in-assembly window and when only in the in-assembly.

Only time I can think of that I can't is when I preselect on the "select component item" or "select assembly item". Then it only allows for the one I preselected.

[cid:image001.png@01CF3EAA.8F579D80]



I miss the mate/align/insert differentiation in the constraint. When I am redefining constraints and I have 3 coincident constraints, it takes an extra click or 2 to figure out which one is which. I think it's more of a nuisance to me. Just seems like something got lost in translation.

Steve


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

I like the double window best. Have gotten use to single though. But what I don't like is if you have the other part open in a window then it pops and completely hides your assy window. Then clicking back and forth is a mess.

What I would like to see returned is the multiple select on one part option. It was a while ago maybe in WF2. You could assemble a part, and window would pop up say a bolt, then you could pick the diameter and at the same time also pick the flat under the head, then go to the assembly window and pick the hole and then the flat surface and boom you were done. No back and forth.

Ron

Query Select in Creo?

Hi all - I'm starting to get off topic here - but consider adding interface
features to your bolts - etc. (component interface - in WF5 it is considered
a datum feature - insert>datum>interface - in Creo it is in the Model tab on
the right.) Then, when assembling a bolt, you only need to pick the hole
cylinder, and the mating face in the assembly. Boom - done. The fastener
knows what it needs to assemble itself.



There is even some form of assumptions built in that is supposed to see
what's on your screen and automatically assemble the fastener - I have seen
Creo try to do this, but it has never been successful. Not in Creo now, so
I don't know the terminology for that. Anyone use it and like it?



-Nate


Query Select in Creo?

I just choose a bolt as an example. We actually have interfaces set up so even for me assembling a bolt with the dragger on is not an issue. It was an easy to understand example everyone could quickly grasp.

Now our cad-admin had set up the automatic assembly also by default. Works when you test it on a small assembly as I am sure he did at the time he decided it was a great idea. BUT, and oh what a big BUT is it, try assembling that bolt in to a large assembly with several 1000 components and several 1000 holes. It took me a week or two to figure out that it wasn't just CREO that was slow, it was our new and improved bolt assembly technique.

Steve

Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Query Select in Creo?

That's why we try to use functional sub-assemblies as much as possible.
On a tooling assembly for example, we may have a common punch holder plate that is only one part model, but also has an assembly with the same p/n showing all of the preferred assembly components, fasteners, etc... to be used as the norm. On the part drawing, there is a second sheet showing the plate assembled along with the preferred hardware.
Along with skeleton models, it really simplifies large assemblies with lots of parts.

Christopher F. Gosnell

FPD Company
124 Hidden Valley Road
McMurray, PA 15317
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