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1-Visitor
Sep 25, 2012 7:35 PM UTC
Question

Assembly rounds?

Good afternoon, All:



I have a part that will go through two stages of machining: the first will
be a blank for waterjet; the second will add blind cuts. To do this, I've
made the waterjet blank, assembled it into a new blank assembly, and made my
blind cuts. I would like to put a round at the inside edges of the cuts
where they meet the next surface, so I go to Cut & Surface>Engineering>Auto
Round> Round. But nothing highlights as I mouse over the model, and I can't
pick any edges or surfaces to reference for the round.



Can anyone tell me what I'm missing? Is there a configuration option I need
to set?



Creo 2.0 M010/Windchill 10



Thanks,



Carol



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef


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19 replies

1-Visitor
Sep 25, 2012 7:53 PM UTC
As long as I can remember, you haven't been able to add rounds in an assembly. Because depending on where you add them, you could be actually adding material, which in a Pro/E assembly is never allowed.

Tim Knier
QG Product & Support Engineering
QuadTech
A Subsidiary of Quad/Graphics
Sussex, Wisconsin
414-566-7439 phone
-<">mailto:->
www.quadtechworld.com<">http://www.quadtechworld.com>
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1-Visitor
Sep 25, 2012 7:57 PM UTC
Get rid of the assembly.

Create your waterjet version. Publish geom the quilt.

Then make a new part, copy geom the waterjet as first feature.

Make holes. Make rounds.

On Tue, Sep 25, 2012 at 2:53 PM, Knier, Timothy <-<br/>> wrote:

> As long as I can remember, you haven’t been able to add rounds in an
> assembly. Because depending on where you add them, you could be actually
> adding material, which in a Pro/E assembly is never allowed.****
>
> ** **
>
> Tim Knier
> *QG Product & Support Engineering* ****
>
> QuadTech
> *A Subsidiary of Quad/Graphics**
> *Sussex, Wisconsin ****
>
> 414-566-7439 phone
> -
> www.quadtechworld.com ****
>
> ** **
>
> *From:* Carol Fly [
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cfly1-VisitorAuthor
1-Visitor
Sep 25, 2012 8:06 PM UTC
Yes, that's the way it used to be. But if you wanted to make an assembly cut
with a ball-end mill, it would be rounded where the cut met the new surface.
And Creo has this functionality, but I can't get it to allow me to pick
anything.



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef
Translate
cfly1-VisitorAuthor
1-Visitor
Sep 25, 2012 8:12 PM UTC
Some people are suggesting that I merge the part into another part and do
the round there, but external references are strictly forbidden in our
organization, so that's not an option. The only workaround I see if I can't
get this feature to work is to pull the assembly cut back and make a swept
feature to cut the round around the edges of the cut. But I've even tried to
do that, and can't get to a point where I can define the section to sweep.
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1-Visitor
Sep 25, 2012 8:17 PM UTC
I think the rounds you describe will add material to the part. If they
are assembly features, they can remove material only.



Why not make the item as a part with a family table for the
configurations. The generic part would be waterjet blank with blind
cuts. The family table would have one instance waterjet only, the other
waterjet with blind cuts. Add parameter data for each instance to
control things like part number, description, etc...



I do this for forgings, and also machined parts in various stages (ops)
of prismatic machining.





Christopher F. Gosnell



FPD Company

124 Hidden Valley Road

McMurray, PA 15317
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1-Visitor
Sep 25, 2012 8:40 PM UTC
Create a family table: 1 instance with rounds, 1 without.


On 25.09.
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1-Visitor
Sep 25, 2012 8:46 PM UTC
FYI - Proceed with caution: PTC has changed how family tables work as of CREO1.0... the whole family table is treated like a single file. Generics and instances cannot be revised or released separately depending on your OIR rules.

This messed with us really bad and thought that I would mention it.

Michael Ohlrich, Design Engineer
Benchmade Knife Company
mohlrich@benchmade.com<">mailto:mohlrich@benchmade.com>
(503) 655-6004 x122

[cid:image002.jpg@01CD9B24.2FA123F0]
www.benchmade.com<">http://www.benchmade.com>

CONFIDENTIALITY NOTICE: This e-mail communication and any attachments may contain confidential and privileged information for the use of the designated recipients. If you are not the intended recipient, (or authorized to receive for the recipient) you are hereby notified that you have received this communication in error and that any review, disclosure, dissemination, distribution or copying of it or its contents is prohibited. If you have received this communication in error, please destroy all copies of this communication and any attachments and contact the sender by reply e-mail or telephone (503) 655-6004).
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cfly1-VisitorAuthor
1-Visitor
Sep 25, 2012 8:49 PM UTC
Yeah, I'm not apt to use that approach either, as family tables are frowned
upon for this kind of thing. We, too, have been burned by them.



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef
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1-Visitor
Sep 25, 2012 9:02 PM UTC
I don't want to sound rude or too argumentative, but here are the two
situations you have;

Your method with assembly features

Object 1 is the waterjet part. It exists as an individual file
Object 2 is the assembly with your holes. It exists as an individual file.
It also has EXTERNAL reference to object 1, being an external file and an
entity within your assembly.

My method

Object 1 is waterjet part. part file.
Object 2 is part with holes. part file. It contains a single reference to a
stable and controllable publish geom feature.

Both methods contain the same number of file system objects. Both methods
require the existence and reference to an external object for their
creation. There is no file management difference.

However, my method is more stable because you can retrieve and regenerate
Object 2 WITHOUT needing Object 1 neither in session nor in the working
directory. Only if you try to redefine the copy geom does the system need
to retrieve Object 1.

It is a superior method than assembly features in every way for your
situation.

Or as others have said, use a family table.

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1-Visitor
Sep 25, 2012 9:03 PM UTC

Rui -


RE: " but external references are strictly forbidden in our organization.."


That's too bad, because the inheritance function is really powerful and has only one "layer" of externality.


We create net shape forgings or sand casting parts, then create a new machining part with an inheritance feature.


The new machining part (with all the machining characteristics) inherits the net shape forging (or "waterjet" e.g.).


End result: Only two parts are created that need to be controlled.


"Inheritance" does a sweet job of keeping the 2 modeling (process) functions separate: casting (or "water jetting") and machining. Just saying.


~John F.


DRS SSI

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