In almost 20 years of using PTC 3D modeling, while there have been extraordinary gains in capabilities and productivity, there are some limitations I have always had to live with. In this case, maybe some discussion will shed some new light.
All I want to do is to use the same part in an assembly - in mirror dependent locations - without having to create mirrored references or write relationships. Seems simple enough - maybe place a bearing mounting plate on both sides of a symmetrical conveyer for example. Does anyone else out there run into this simple scenario? Personally I strive to use the same part in as many assembly locations as I can - just seems more efficient that way - even though it does require some thought into the symmetry of the part.
Its real easy to do if you can live with having a new part created - but that just complicates the BOM - and the shop is asking 'why did we just have two separate work orders for the same part?'.
First of all, you might think, intuitively, that assembling the same part in a mirror location to an existing part might be an 'Assembly' operation. But no, you have to go through the 'Component Create' interface. Of the 'Mirror types', selecting the 3rd option 'Mirror placement only' will ignore the part name in the previous Component Create window (this is more information than you will find in the Help Center).
The following Image shows the results of each Mirror part 'type'. Both 'mirror geometry' options create the correctly located and oriented part - that also adds another part to a previously simpler BOM. The third option 'Mirror placement only' part is just not oriented correctly - and is totally useless to me. Does anyone else see a problem with this? (Click on the image to enlarge it.)
And yes - this 'placement' can be accomplished with a "Pattern" - but it usually requires a relation or additional references to be truly 'location dependant'.
I have submitted this to PTC and got the response that it "Works to Product Specification". I'd hate to think what would happen to existing model assemblies if a change was made to the current default orientation of any part placed in this way. What I think needs to happen is the addition of an option to control the orientation of the Mirror Placement dependent part - something dynamic on the screen that shows you how it's going to end up oriented.
So I have two questions:
1. How many out there have run into this similar scenario? If no one else does - then I'll quit my complaining and continue the unproductive work of either creating mirrored references (additional Datums) in my assemblies or using 'Patterns' or writing additional relationships.
2. If/When you do run into this senario, how do you handle it efficiently?
Hello Aaron. I got your PM and you may consider putting questions like this in the Creo section. Assembly management seems to draw a different set of eyes.
As for your consideration in making "mirrored" parts that are not true mirrors, but rather identical, indeed I would recommend patterns... but use the point pattern created in a sketch. These can be made very intelligent where the assembly changes, such as moving further from the mirror plane, the points move with the change on a regen. Then the placement is re-evaluated. I love intelligent sketches! Just remember to use the datum point in the sketch. Once the sketch is made, you should see the points if the datum points toggle is active.
As for weird things happening, if only I had a nickle... I can only say that reporting these through loggins support cases is the best solution. Be persistent if something is not happening as expected. A support technician should be getting back to you and they can even follow your actions on your screen in case something needs clarification. Sometimes the case is not evaluated properly and you need a second look. There are escalation opportunities on the support site. I know it is an extra effort, but it really does make the software better for everyone.
There is an upcoming fix regarding patterns in Creo 2.0 M090. I am very much looking forward to it.
I know you know the drill after 20 years. This falls under "technique". I do like point patterns... when they work. I also have a habit of selecting "pattern origin" rather than letting the system evaluate one.
You mention an old known functional gap, that can be defined as "mirror assembly and reuse symmetrical parts, smartly locating them in mirrored assembly". I have no legal to commit, but this is on a to-do list for our next version to come (not the one in current development, unfortunately).
We do have an old option to say "Reuse" for some components while in Assembly Mirror UI (or if you just mirror one part - option "mirror placement only"). What it does it simply "mirrors" part origin vs. the plane and sticks reused part by its origin to that mirrored CSYS. Now : when CSYS is mirrored we have to flip one of its axis to stay in Cartesian system (right handed CSYS) - and Creo steadely will flip Z direction if I remember it correctly.
Now knowing this you can design your symmetrical parts in a way that will work just fine for such Mirror / Reuse : design a part symmetrical vs. X-Y plane, try Mirroring it - see what happens. In particular for bearing which has 3 planes of symmetry it will be enough to model it when midpoint of the bearing coincides with model origin.
This might be not relevant proposal if you already have designed parts or imported parts that have their origin far from symmetry plane ...
Let me know if you try this and it works
I am just reading your post. And yes I am flabbergasted; after finding out that I was unable to perform one of the most simplistic operations in Assembly mode that should exist - The Mirror Command.
Still to this day, evidently the only way to perform this operation is through the Assembly Create Component and put-up with creating a whole new, separate part number installed where you want the same one from the existing Model Tree BOM. I am using Creo Parametric 2.0 M100.
Somehow I remember though that many years ago, in some versioin of Pro/E you could do that. Mirror a component in Assembly mode.
I find it very interesting that after 1627 Views (to date), only three commentaries on the subject. Oh well.
You can mirror a part that is not a new component using Create. It is the terminology that PTC uses and that you have to give a "new name" that cause confusion. Aaron is having difficulty with some quirks about the way Creo is mirroring the components. I haven't experimented with Aaron's scenarios and can't comment on them.
To create a simple mirror placement of a component in an assembly, in the Model tab, select Create then in the next box, select Part and Mirror (give a name for the part that will not be used but is unfortunately the confusing part), then select OK. In the next box, select MIRROR PLACEMENT ONLY (this is how Creo knows you don't want a new component even though it made you give a "new" name) and then select the component to be mirrored and the mirror plan reference.
This method is NOT creating a new component and your BOM will be accurate.
It seems that "mirror placement" only rotate part around vertical virtual axis which is on symmetry plane. Is it possible to rotate (mirror) part around virtual horizontal axis in the same way?
Well, some good news : finally and after long processing (I admit too long) Component Mirror will get serious revamp ... in Creo04.
This will include recognition of symmetrical components (parts and assemblies), their "smart reuse" upon mirror operation, and also user control upon "Mirror Placement" option in a non-symmetrical cases (select axis to be flipped upon Mirror).
I know that Creo04 sounds a bit far to you, but at least there is a "V" in our "To Do" list.
New Component / Mirror capabilities were shown off at latest Stuttgart user event and got good responses.
p.s. my earlier post in this thread actually explains how to avoid issue that Aaron mentions in the initial message (how to design symmetrical parts so that Mirror / Placement Only option will work as desired). I did not hear any comments on that proposal though.
Vladimir Zak wrote:
... I know that Creo04 sounds a bit far to you, but at least there is a "V" in our "To Do" list. ...
With Creo 4 due in about a year, then another year for my clients to start using it, I'm looking forward to using this fix sometime in 2018.