Sharing Sketch in Assembly

[tfhall]

 Why can I not share a sketch in when I'm working on a part that is featured in an assembly?

For example, I'm trying to use another part's geometry to create a new part. When I'm working on this new part in the assembly, it for some reason does not give me the option to share a sketch. This doesn't make any sense....

Any help?

[admaiora]

Hi Tfhall,

no you can't share a sketch between parts, not in the way you are trying.

And that has sense.

You can derive a part and his skethes while creating  a part.

Or you can project geometry while modeling a part in a assembly (adaptive geometry...pay attention with this way)

[johnsonshiue]

I think you are talking about not being able to share Adaptive Sketch. The reason why it cannot be shared has something to do with Adaptive technology itself. It prevents two things from happening.

First, if an Adaptive Sketch is shared, the features consuming the same sketch may not obey compute order. For example, Exrtusion1 consumes AS1. Then AS1 is shared and it is consumed by Extrusion2. If Ext1 and Ext2 are totally independent, sharing AS1 should be fine. If Ext1 and Ext2 have dependency or associativity, Ext1 could be driven by Ext2. It is because Ext2 is also an adaptive feature freely to be influcenced by geometry from other components or assembly constraints. The problem here is dependency and associativity might be established before or after the sketch is shared. There is no way for Inventor to prevent this from happening. As a result, Adaptive Sketch is blocked from being shared.

Second, it is to help preserve compute stability. Let's reuse the above example. Let's say Ext1 and Ext2 are totally independent (deleting Ext1 will not affect Ext2) and they just share AS1. Now, a side face of Ext1 is driven by Constraint1. The same side face of Ext2 is driven by Constraint2. Unless the two constraints always have the same effect (same distance or same angle) on the body, should Constraint1 win or Constraint2 win?

I am sorry to write a verbose reply but there is indeed some limitation in the technology itself. In theory, it is possible to unblock the limitation with very intricate logics built behind to scene to handle various complications. But, the behavior will also be confusing and hard to understand.

Thanks!

[mikeh4]

I also would like to see this and understand the circular association involved.

Can we open it up so if it's non adaptive geometry we can share the sketch?

Quite often we'll have a raw part, some times a casting or forging, as an ipt and then machine it as an iam and when doing bolt patterns it's nice to have 1 sketch w/ all center points and via share sketch multiple hole commands.

Thanks!

[johnsonshiue]

Hi! I think you are talking about sharing assembly sketch. We have heard about this request for a while. Unfortunately, it is not done yet. I hope it will be enabled soon.

Thanks!

[kmeldfreyssinet]

@johnsonshiue

Hi Johnson,

hope you are still subscribed to this thread.

I had just needed this functionality (to share sketch in assembly. I wanted two extrusions from one assembly sketch).

I wish to inform this is still not implemented and it is now 2016.  This functionallity really is expected in some real life cases.

Cris.

[dan_inv09]

It is very annoying when basic (you might even say essential) functionality from one environment doesn't work in another.

(Right now I'm making a bolt hole pattern in an assembly that is not going to be recognized to pattern the bolts.)

I haven't really paid enough attention to see how well it really works/adapts, but I just project from the one sketch onto a new sketch.

That's just a workaround, I'm not letting anyone off the hook for sloppy programing - although I suspect it is not the programmers fault, it's poor management: this sort of systemic ineptitude filters down from the very highest levels of the organization. People who believe high executive salaries and bonuses are necessary to attract and keep the best and brightest haven't really looked at what they're getting lately.

[kmeldfreyssinet]

There is plenty of such "inconsistencies" in Inventor and it seems no one is interested in doing anything with it.

I used to wander if Autodesk has people that try to use Inventor in real life projects, just basic ordinary, average projects and uses their feedback to improve those little stuff that makes you suffer.

If missing of essential functionality or most basic bug is reported there is no way to find out when and if it will be fixed.

There is this "Idea Station" but there should be "Bug Report forum" that would get much more user involvement, as lack of possibility for using basic functions that are said to be implemented, but are not working, is much more of interest of users than new features that are not even there yet.

Cris.

[johnsonshiue]

Hi Cris,

We are aware of the request and we understand the need. It does not seem as straight forward as it appears. I will follow up with the project team.

Thanks!

[kmeldfreyssinet]

Hi,

Original post is from 2014. Now is 2016 and since then Autodesk had introduced many changes not only in to inventor but also to other its programs.

At least many of those changes are significant and in some cases require redesigning parts of the software totally.

So it is really very hard to believe that not fixing known bugs or limitations is only caused by technical problems.

My self, and I expect also other users, see the cause rather in lack of will to do it than in technical difficulty.

I admit there are some bugs fixed and some limitations removed during years. But also in the same time other are introduced. Nevertheless general Impression is still that it takes much to long to remove known bug from the software.

Cris.

[SBix26]

I think what @johnsonshiue is saying is that this is much more involved than fixing a bug or a simple "just do it" type of project.  As with any business, finite resources get allocated to only some of what needs to be done, and the allocation decisions don't please every stakeholder.

I haven't seen any reference in this thread to an Inventor IdeaStation posting.  Has anybody done this?

Sam B

Inventor Professional 2016 R3 SP1 Update 1
Vault Basic 2016 SP1
Windows 7 Enterprise 64-bit, SP1

[mikko.m]

Here is one idea that I found

[ToddHarris7556]

I'm not hating on/dismissing anyone's specific need, but perhaps one reason it hasn't gotten a lot of attention is that there just aren't a lot of people seeing it as a problem. 

As a designer, I would not see bolt patterns like this as appropriate to leave until the assembly stage to lay out. i.e. Skeletal modeling workflows have been around for.... well, decades. We use master models to control key interfaces, and then derive those control points as needed to generate parts. If it's a shared bolt pattern, I can see it being developed in a skeletal model, and I can also see that it would be legit to model the pattern in one part, and then simply create an adaptive part in the assembly that projects of this geometry. (Note: I'd say most folks would lean toward the skeletal model, and try to minimize adaptive parts where possible as a best practice... but it can, and is, done all the time)

I guess all I'm suggesting is that out on the shop floor, it would seem like a little bit of an unnatural act to have two raw blanks show up in the assembly area, and to do the bolt pattern layout there. That seems like what we're trying to do in terms of this electronic workflow. It would make more sense to me to either send a print out, and have both bolt patterns machined when the parts are made (skeletal modeling) or have one machined, and one show up blank so the pattern could be laid out with transfer punches. (Adaptive). 

Just my .02. 

[dan_inv09]

The specific "bolt pattern" issue was not transferring holes from one part to another. It was that a hole pattern created in a weldment was not recognized to pattern the bolts. It was not the OPs issue - we do not know why tfhall needed to share a sketch - the "Feature Pattern" not recognizing assembly features was simply another example of functionality that doesn't work the same in an assembly as it does in a part.

It does not matter what it was needed for, it does not matter if the workflow makes sense. A sketch is a sketch - someone is used to sharing sketches in parts so, "It would be convenient to share this sketch here ... wait, why can't I do that? Does share sketch not work because I'm in an assembly? Almost everything else to do with sketches seems to be the same as in a part. It is frustrating that this one thing not the same when I need it!"

I was just referencing something else that is different whether it is created in a part or an assembly - and on the floor, some holes need to be drilled after the parts are welded together (especially if the important faces are going to be machined as well). But enough about Feature Patterns for bolts, that has very little to do with sharing sketches in assemblies no matter how elegant your workaround may be.

[ToddHarris7556]

Fair enough. 

Without a part, or a screenshot, I may have completely misunderstood the OP's need. 

I often have clients request things that I think are unnatural acts. The requests make perfect sense in their minds, because they're not engineers. While some of the requests may be *conceivable*, that doesn't mean they're good engineering practice. It's my responsibility to suggest options that are safer, more cost effective, and/or more functional. That doesn't mean I don't respect the fundamental design intent/request, it just means that I have enough experience to know that they're asking for something that's not considered sound practice. They can either consider my suggestion, or go about their way with my very best wishes. 

I was simply offering a perspective. It sounded to me like the OP was asking for approaches to a problem. I shared what many consider to be best practice, with complete respect for what I understood to be the end goal. 

******************************************************************

If I stop off at the lumberyard on my way home and ask someone to help me duct tape 6 sheets of plywood to the roof of my Smart Car, I would fully expect that someone tell me that's not a good idea. Whether I choose to listen to them or not is, in fact, my choice. 

[Frederick_Law]

If you need to share sketches between parts and assemblies, use master sketch work flow.