Assembly rounds?

[cfly]

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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[TimKnier]

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>

[lococnc]

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 [

[cfly]

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

[cfly]

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.

[ptc-1932745]

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

[ptc-2032585]

Create a family table: 1 instance with rounds, 1 without.


On 25.09.

[MIchael_Ohlrich]

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).

[cfly]

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

[lococnc]

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.

[Tundra]

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

[cfly]

This was apparently meant for me, not Rui.



By using the waterjet blank as the only component of an assembly, I, too,
have only two files to be controlled, and the blank is automatically brought
in when the assembly is opened as the base part to cut; this is how we do
all of our "altered items." The only reason this is a problem is because I
cannot add a round to an assembly; it has to be a swept feature. But I feel
the round functionality should be available in assemblies because there are
many times that a cut might be made after assembly (particularly in a
weldment) that would be created with a ball end mill, and therefore, the
round would be there - in reality, it would not be adding material, even
though it does that in the file when the operation has to be done with two
features.



Either way, it's not my call to change our policy.



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef

[JonathanHodgson]

Carol,



Could you create your cuts as surfaces (quilts) first; round the quilts;
then solidify as cuts?



Particularly for ball-ended cutter features, and milled pockets which
break out through complex geometry, this technique can be more stable in
any case.



Jonathan

[merrill.rosenow]

In Reply to Carol Fly:

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.

How are family tables bad for this kind of thing? It would have been the first thing I would have suggested:

Make the generic the final version of the part after machining is complete. Make an instance called "filename_waterjet" or something like that and suppress the rounds. You can now put these two instances into one (or two drawings if you are so inclined). The easiest example of where something like this occurs is with sheet metal parts. The blanking is done on one machine, then the forming is performed on another. Both of these instances appear on our drawings and are used to make the final part.

How do family tables burn you? I'm not sure why it wouldn't be the most robust way to deal with this. It was also mentioned that Creo's method of treating an entire family table as one file would revise all instances. We have always updated all of our instances at the same time like this, and besides it being potentially inconvenient for certain people/companies (having to potentially update physicaldrawings on the floor) I'm not sure why this would be a problem either?

[cfly]

That's a thought; I'll have to try that next time I have something like
this. Thanks!



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef

[cfly]

The problems happened before I came here and for a little while after,
before I was up to speed on things, so I didn't experience them and don't
know the details. Honestly, they might have been exclusive to family tabled
*assemblies*, but I'm not sure. The rule here has been to avoid them when
you can except for library parts, so I do, and the single component assembly
with assembly level cuts is the way we've been told to do altered items, so
that's what I did. That's all I can tell you; perhaps someone else from our
organization can elaborate...



efefefefefefef

Applied Research Labs

University of Texas at Austin

Carol Fly

Mechanical Designer

(512) 835-3397

Fax (512) 835-3259

efefefefefefef

[jbennett]

We use family tables for our processed parts (like bent brackets, etc.). They do work well in many instances, but if you use Windchill or any type of promotion process to control your parts, you have to have the change process defined to make sure that all of the instances are revised (changed) at the same time. If you don't you will run into issues on the backend of the storage (check in issues, etc.)

Just a thought on family tables from the administration side of things.

John Bennett
Cad Business Administrator
(801)513-9001

[Lifetime_Logo_BlkWhite_Sans_email sig]

[nrollins]

My solution would be to create the cut geometry in the assy as a surface
quilt (including rounds) and then cut>use quilt (solidify).

[mkelley]

This is a perfect application for inheritance features, IMHO.

First, design your finished part. Be certain to model it such that the interim steps appear in the proper sequence during the part history.

Next, create a model for your 2nd manufacturing process; inherit the finished part geometry into it. Edit the inheritance feature, and suppress the blind cut features created by the 2nd process - et Voila, you will have your post-waterjet part!

Copy this part - it will become the model for the initial waterjet blank. Edit the inheritance feature; supress the waterjet cuts - and you should now be left with your blank part.

I don't think that this will cause you any Windchill or Creo-related grief, since no Family Tables were harmed during the making of these models!

Good Luck and let us know if it works...

In Reply to Carol Fly:

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

[BrentDrysdale]

Hi Folks,
I endorse Mark's proposed methodology. Of course in ProE there are
numerous ways to achieve the same looking result so to me it boils down to
robustness and I think Mark's method is the gold standard.
Sure you could do it all in one model with family Tables and for simple
stuff this can be robust however it can spin out of control if you get
variants or change in design.
Personally I do not think assembly cuts are a robust methodology and we
don't use them for that reason but in the end nothing is right or wrong.

One caveat in my comments is that we still don't yet have PDM with the
additional complications which that can cause but I wonder which of the
three approaches is most robustly handled in Windchill? I saw a very good
presentation back at the 2007 conference by Kevin Anderson and Craig
Iverson (Of Fluidmaster) on using Inheritance Features versus Family Tables
for use in Windchill and I was convinced. I can find a PDF of that
presentation if people are interested.


Regards,

*Brent Drysdale*
*Senior Design Engineer*
Tait Communications