In-place assembly editing

[DaveWilliams27]

Hi, when editing a part in-place, why is it that I can't dimension from or snap to other parts in the assembly? Another example is if I want to make a hole in an assembly, I can't dimension from any faces or parts in the assembly.

In the following video, he is able to edit a part by snapping to other features in the assembly. I can't do this. Any ideas?

http://www.youtube.com/watch?v=eGLfpDwN0vo

 

[DaveWilliams27]

I can't even use the steering wheel to snap to features of other assembly parts for positioning them, like in this video:

http://www.youtube.com/watch?v=SzhmMc4uCpU

Clearly there is a setting I'm missing somewhere.

 

[kjoiner]

Hi Dave,

Are you working in the Synchronous or Traditional(ordered)method? If you are working in Traditional and have your controlling sketch or features in the assembly you will need to use the include edges command and check "maintain associativity" in the dialogue box. Alternately, if you are editing a part and want to place a dimension that locates a feature relative to an edge, face or other feature of a part in the assembly, you can pick the "peers" option under the "tools" tab while you are creating a feature. Here are the steps:

Using Include
1. Edit your part from the assembly. If you can't see the assembly, use control+Q to show it
2. Start a sketch or feature
3. Once you are in the sketch, pick the "include" tool in the "draw" tab. Check "maintain associativity" and select edges etc to create the feature or constrain it.
4. Solid Edge will inform you that relationships have been created between the assembly and the part

Using Peers
1. Edit your part from the assembly
2. Start a sketch or feature
3. Once you are in the sketch, pick "peers" under the "tools" tab and turn it on. You can now dimension from peer edges or constrain geometry to them. Make sure the parts in the assembly have been activated.

Hope this helps.

Kyle

 

[DaveWilliams27]

Hi Kyle, thanks for the help. I always use the Synchronous method when it's available. I tried your steps out in the Ordered environment, and turning on "peers" unfortunately did nothing to make other parts available to dimension or constrain from. The other parts are visible, but their visibility is faded - almost wireframe.

I also tried the "include" tool, which did work, I was able to create a new sketch based on features from the other parts, but since I'm unfamiliar with the Ordered environment I'm not even sure how to use the sketch to create features.

I just can't understand why I'm unable to do the things demonstrated in the videos on my installation. I can't even use the wheel to snap to the base axis for repositioning with respect to the base axis. :S

 

[DaveWilliams27]

Ok I see I can transfer the sketch to the Synchronous environment where I can use it normal. However obviously this is a work around and not how the program should be able to work.

Oddly, I'm able to use the extrude command to select peer part faces without any problem.

 

[kjoiner]

Hi Dave,

I do a little work in Synchronous, but there are others who may be able to provide a lot more detail on assembly modeling with Synchronous. Try posting on the new public Solid Edge forum as well. There are some Synchronous power users who can probably help out. By the way, when you are editing a part from an assembly, and you show the previous level (the parts in the assembly) they will show up as more transparent so you can focus on the part you are editing. Are you new to Solid Edge? If so, welcome to the group. I think you will find a lot of users willing to help out.

http://community.plm.automation.siemens.com/t5/Solid-Edge/ct-p/solid-edge

Kyle

 

[DaveWilliams27]

Ok thanks Kyle, I'll have a look on Monday. I'm quite new to SE yeah, have been using it for a few months but there is still lots to learn.

 

[kjoiner]

Dave,

Keep the questions coming. I'm always glad to help where I can.

Kyle

 

[beachcomber]

Make sure the parts are activated.
You can't locate edges or faces of inactive peer parts.

bc.
Core i5-3570 @3.4GHz , 8GB RAM
Quadro FX4600. W7 Pro 64-bit.

 

[jettocrack]

I usually use the "Peers way", however, I can't get intellisketch to work properly. As an example: I can add a line and then constraint it with relationships to some vertex in the assembly, but those vertices won't be available while drawing it. This makes the whole process a bit slower.

As a personal experience, I try to avoid having features on parts linked to geometry on the assembly, since a number of times, changes in the assembly don't flow to the part so easily, and the whole design not always gets correctly updated. You have to open/close/update/activate etc etc... in the assembly in order to (being lucky) get a full update in the parts. When the lack of a proper update is not easily noticeable (let's say some holes moving 1-2 mm from their theoretical position) you can get into serious problems.

Some other times, the part "loses" those references from the assembly by no logic reason and you have to re-link the geometry

When two or more parts are very related in their geometry, I prefer to use Part Copy with the Construction Body option, thus placing a reference copy of one part inside another. With this way, you don't need a "parent" assembly in order to get the information flowing from the parts. Also, you can import curves and surfaces.

From my experience: In my work, we make complex welded assemblies with curved sheets and any kind of components. I usually select a main part, in which I place the general dimensions which will drive the whole assembly, by means of curves and surfaces (placing notes and so, in order to build a very logical and intuitive model), along with the geometry of that first part. Next, each component will have this part copied inside it as a reference, most of the time copying just the needed geometry/surfaces/curves each part demands, and modeling it just with that info and the lesser new dimensions possible. With this way you can use "Match coordinate systems" in order to build the assembly once the parts are finished, so less work here too. Most of the time, just editing the first part you can get the whole assembly follow the update with REALLY no issues. I'm talking of assemblies which easily surpass 50-100 parts, so you can be sure the result is simply impressive. I tried the same in the past but linking those parts through the assembly and the result was not good, specially when you don't know why a reference has been lost when nothing has changed.

From my experience too, I try to avoid assembly features whenever they are not indispensable. The fact is that I always get all sort of problems and issues when there are sketches which rely upon assembly information, and you have to re-link and re-do, and re-associate whenever measures change in the assembly (just measures, not other changes which could explain those issues), most of the time with no feedback of what has happened.

My apologies for this long post, hope it helps someone.