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config.pro option solutions this problem: auto_constr_always_use_offset never
Since Creo2 release, the default choice when assembling two axes is now "Distance".
I think that the default choice (most often used) should be "coincident."
Why can't you just put a distance of zero - isn't that coincident?
A dimension of zero will be useless in 99.9% of cases!
I'm wasting time to change this dimension to zero in the assembly. The zero dimensions will appear unnecessarily in the drawing.
No, it is not the best practice to substitute a coincident constraint with a zero dimension.
Okay, Nicolas... I have to ask: How do you get so many votes so quickly on your ideas?
Illustrated ideas are often better understood and users probably like them. It is part of my responsibility at Richemont to promote them and influence the PTC dev. With the ideas concept, we were able to obtain evolution in the software. Thank you for your regular votes. Nicolas
ps. it is not easy to write technical concepts in English when it is not your mother tongue.
Agreed, was telling my VAR this last week. Default to distance makes no sense.
Thanks Matt !
last comment to Antonius's remark,
When I work on the migration of new versions of Creo or PDMLink, I often open calls at PTC and when I get the response "work to specs," I create a idea.
I have been using PTC products since 1991 and I really want to influence the software changes intelligently. The ideas are real levers to influence PTC.
Some of my old “requests for changes” hang for about 10 years in a no man's land at PTC. Since the ideas concept emerged, I think we can more be heard.
I was wondering if you send out a "please vote for this" notice to a select group. I have seen very well versed strong ideas that simply get overlooked. But you have 10 votes within a day. That is highly unusual.
As today, I just put a new idea in and I get 4 immediate emails back from PTC saying people are not available. You just know that when they get back from vacation, they will just glance at these unless it has community attention, if then.
Maybe you can support my idea here: Floating GENERAL Toolbar
I support a lot of your ideas
Yes you do, and thank you
Hey Antonius, have a look at how we vote (VERY often) in Switzeland ...
It is an integral part of our DNA
This option solutions the problem:
In reality, the "new" assembly interface as described in the "enhancement" videos -suggests- that the "improvement" includes -intelligence- by knowing if the object is close to the references or if it is -at distance-. So if the object is close together, then it will pick coincident, but if they are at some "significant" distance, distance will be selected.
Good find! I already set it and tested it.
Yes if they were close it would go coincident by itself. But that seems to be about 5% of the time for me. I am sure if I spent the time to move the part closer to the point of assembly it would work that way, but the time spent doing that would probably be even greater than changing distance to coincident.
Even though you found a workaround to this that works very nicely, I still voted for it just to let PTC know that keeping this config option is important as I don't want them to remove it in future versions!
@NicolasBourgeoi1, @TomD.inPDX & @Inoram
When we first went to Creo2 I tested this and other config.pro options extensively because this is a very annoying problem for us who primarily use semi-rotationally symmetric models. There are also some options for them to conditionally coincide or stay oriented/offset. However, the config.pro really needs to control axis and datums independently of each other.
For rotationally symmetric parts you usually want to constrain to the center axis while often offsetting from a datum (or surface)...such as using an oriented constraint. However, if you use this option it shifts the annoyance to moving your part from being offset to coincident and you will either loose your approximate location or cause an error. Of course there are workarounds to all of this but the way it is done now is slower than what it used to be, and it is a highly repetitive action.
I like having the option, but it seems the vast majority of the time axis are used to coincide with stuff, not be oriented/offset. I am curious, if you have used the orient/offset constraint before, what have you used it for? I am having a hard time imagining the cases it is useful (although I am sure they exist)
I occasionally use offset from axis, although usually it is during the design process more that during the production process simply because I can place and adjust a component location based on the axis without adding a feature to another component, ie. I'm trying to figure out placement of a component and I'll add the mounting for it at a later time. Occasionally I will need to place something at a distance from a hole (axis of the hole) and that specific hole doesn't have datum planes, you can use the axis along with default plane to fully place a component.
I use the option above (auto_constr_always_use_offset never) since most of my parts are coincident via axis and/or planes/surfaces and rarely am I offsetting (with the exception of the design/layout phase).
I do find it very annoying that when I have an offset constraint and I redefine it, it will change the constraint to coincident (based on the config option) if I don't specifically reset the constraint to offset.
Not only does it change to coincident, it teases you with the number in the box grayed out and you changer the constraint type and it loses that number and sets it to zero. Yes very annoying. At least Creo2 does, I am not sure about 3+.
As far as the other question, I am not 100% sure I understand but I use parallel or angle when rotating on axis.
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