Assembly mode cuts and chamfers in Creo 2 M50

[Beyontech1]

I am looking to create several cuts and thenbreak the edges with a chamfer in assy mode.

I created the cuts and select the edges and the chamfer icon is greyed out.

Did we loose functionality in Creo? (I just updated from WF4)

[StephenW]

Chamfers and rounds have never been available in Assembly mode.
The reason according to PTC is that they have the ability to add material (think of the internal corner chamfer or round) and in an assembly, you can only add "material" by assembling parts (or assemblies).

I guess it's a valid reason but I really don't agree with it.

[BenLoosli]

Create a sketch of your cut with the chamfers and then subtract that in assembly mode.

Adding material in assembly has always not been allowed. IF the software was intuitive enough, it would know the difference between an add material chamfer/round and a subtract and allow the subtract in assemblies.

[laura.woodward]

thats a high horse ptc is sitting on. its sounds as if they intended proe to prevent you from modeling things you cant create in real life. the last time i checked, i could still create features that can never be machined or formed by currently available manufacturing techniques.

creation of rounds is not really adding material when youre making a cutout or adding blind holes at the assembly level (on a weldment for example), and you want to accurately represent the fillet radius at the bottom edges of that cut/hole.

in a past life, i used to curse ptc's name every time i made a counterbored hole in a weldment, because i couldnt add the fillet radius after the hole. as i work-around, i put the hole at the part level, which required the duplication of relevant assembly datums in the part for gd&t control. when features like blind holes and cutouts are machined and controlled at the assembly level, they should be able to be modeled there, fillet radii and all.

its been forever since i had to deal with such things, but im disappointed to hear creo2 still has that limitation.

Laura Woodward
Senior Mechanical Engineer
Saab Training, LLC
Orlando, FL
(407) 281-3012

[Beyontech1]

Thanks for the input,

It seems stupid that I can not use a time saving chamfer command instead of rovolve and etrused to create the geomotry that can and is done every day in a simple machine operation of an assembly.

I swear I could do it in WF4 but I have now way of checking now.

[StephenW]

No, unfortunately it has never been available. I'm running WF5 currently and the chamfer and round icons are greyed out.
I remember that this has been a complaint of mine since pro/e 15/16 way back in 1996.

Anything other than a simple revolve cut or straight extrude can become a nightmare sweep that will cause problems from the day it is created until the day the part dies. At least that is my opinion.

Our method here at NOV is to use a merge technique when we are going to do "complicated" machining on an assembly (usually a welded assembly) to make the assembly into a part. It is prone to certain problems also but when you need to machine a large welded assembly, it's what I would consider the lesser of the evils.

[mpeterson]

And why not put the feature in the part file?

Regards,
Mark A. Peterson
Design Engineer
Varel International

[Beyontech1]

In short the features need to be machined when the upper and lower components are mating to create a continuous surface regardless ofmanufacturing mismatch.

The feature cannot go in the part file because the forging and machining are done at manufacturer A.

Then it is shipped to a second manufacturer B who heat treats and additional operations after the part is assembled.

Manufacture A and B each have individual drawings.

[daniel.garcia]

For more complicated rounds do like this:
- create surface at assembly level, with copy, for example
- create rounds between surfaces
- merge if necessary to get closed quilt
- create cut using quilt

HTH

Daniel Garcia

Enviado desde mi iPhone

El 06/09/2013, a las 20:05, "Loosli, Ben H" <-> escribió:

> Create a sketch of your cut with the chamfers and then subtract that in assembly mode.
>
> Adding material in assembly has always not been allowed. IF the software was intuitive enough, it would know the difference between an add material chamfer/round and a subtract and allow the subtract in assemblies.
>
>

[JonathanHodgson]

Those of you with active maintenance, log into Planet PTC and vote up this Idea:

[DonSenchuk]

No, you didn't have the ability to do this in WF4. This has always been the way Pro/E has worked. (Well, I can only confirm this is the case for the last 16 years. Our more experienced members would have to comment on older releases.)

[Beyontech1]

I complained to the guys at PTC LIVE GLOBAL 2015.  I am often making band-aids for such features.   Just this week I had a weldment that I put a square o-ring groove into, It sure would have been nice to put a round in each of the grooves.  I got lazy and did not want to create all the surfaces and solidify them.....I just put a note on the drawing and grumbled to my cube mate something nice about PTC.

[ajaynavale2018]

i made a sketch in creo 4.0 & for every corner i have to mentioned the corner radius/chamfer value. it really consuming a lot of time. 

what is the simple way to do in minimum step.

[TomD.inPDX]

It seems to me that family tables lend themselves greatly to manage post-processed parts within next-level assemblies.

I am also a fan of assembly Merge operations if you can manage phantoms on your BOM and/or don't have objections to external relations. 

I am not a -big- fan of either solution though.  On the fly I would go for a simple sweep or revolve cut to solve the problem.

I will cycle through these options depending on the ultimate task at hand.

Also look into welding... -that- was PTC's answer to adding material!

And no answer for raw assembly level deformation by tonnage! 

[Patriot_1776]

It seems I agree with all here in that we should be able to add material (welds) and make simple things like chamfers and rounds at the assy level.  Honestly, why not have access to ALL the modeling features, and then if we make something that can't be manufactured, well, that's on us as it always is here in the real world.

Our spacecraft uses composites (carbon fiber), and there are times 2 parts are joined at assembly with additional layers of C/F, and these can be very complex shapes.  Also, sometimes after adding this extra material at assembly, a final finishing cut is done on the assy as a whole, to get the desired aero shape.   How are we supposed to do that easily if we can't freely add or subtract material????

Ok, if it needs to be a little more $$ in the "Advanced Assy" option, we're willing to pay it..  you listening PTC?