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Basic model management

[ Edited ]

This is a basic question, but I need to ask it.

 

When looking at "occurrence properties" one can toggle on and off:

Reports (Parts list)

Views (Draft views)

Physical Properties (Weight)

 

How do the following switches relate?

Construction

Reference

 

In general, there are three situations I'm trying to handle. I want to figure the easiest switches for each situation. This may need to be answered differently for different types of models: Part, Sheet, Frame

 

1. Normal. It's a part with weight, displays in all view, and show up in parts list

2. The part is only there for easier modeling, only needed at the start of modeling process and is used to link and re-size other parts. No weight, not in parts lists. See through display is preferred when on.

3. The part is there for design room, and does need to display in both model and draft, but is not in the Parts list and should not have any weight. (Even if the part has an assigned weight)

 

I think 2 is construction, and 3 is reference, I cant even find the construction switch.

 

Right now, I just add and delete stuff from models as is needed for design work. Also, I use the "Match"  default solid edge view for all my drawing views unless I'm forced to put holes in a frame part. This has worked well for turning off all the sketches that can show up in draft.

 

32 REPLIES

Re: Basic model management

For 2. I would use Reports: no, Drawing: no, Physical Properties: no.

Occurence props won't control visual style in the model. You'll have to set that with View tab/Style/Face Overides.

 

3. Is essentially the same. Again, display in the model is not controlled by occurence properties except in the case of higher levels, and needs to be controlled by hiding and perhaps configurations for easier management.

If you wanted the part to display in the drawing leave Drawing: yes. and if you want it to appear with reference lines, set Draft Reference to yes. You could control this with the view properties dialog if you want individual control of views rather than a "global" setting. There's usually more than one way to skin a cat.

 

 

Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Basic model management

The key aspect of Reference is that it is a "private reference" at your level of assembly. If someone else in your company were to use your assembly as a subassembly in a higher level, they would not see any reference parts. This is really powerful in a concurrent engineering environment. 

 

not only does it not show, but as of ST7 it doesn't load either --  so you can attach a big honking thing as reference, but when your asm is used as an subasm by someone else it won't carry along the reference.

Dan Staples
Director, Solid Edge Product Development

Re: Basic model management

[ Edited ]

How does one set that Reference value? I only see "Draft Reference" in the Occ Prop dialog.

Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Basic model management

I was hoping for one click solutions, but the matrix of properties is a nice view of what is going on.

 

I'm still wondering where one finds the switches for construction and reference. So I could test them out.

 

If the "referance" is only there for the origionator, then that would be a bad choice as the sizing object of Sync sheet metal models.

 

I'm just about to re-tool all of my models using Sync for the shells of my sheet metal models. All of my shell parts will be controlled by a dummy block that represent the outside surfaces of some shape of sheet metal. That dummy part will be re-sizable and in turn control the size of everything else. Features of the shell, and the rest of the parts will stay in ordered.

 

The goal of re-tooling is to reduce all inter part dependancies to only variables once past the shell & dummy parts.

 

Imics showed me how to use Sync in this way in another thread discussing the move to Sync.

Re: Basic model management

Dan? Where'd you go?
Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Basic model management

Sorry @bshand, just doing my real job for a bit. :-)

 

I peaked and see that we changed what we used to call a reference (or maybe that was just an internal term) to "Higher Level". This is a bit clearer. When checked (the default) it will display the subasm at the next higher level and beyond. When unchecked, it will not display said subasm in higher levels of the ASM. In other words it is private to the current level.

 

Have a great weekend!

DS

Dan Staples
Director, Solid Edge Product Development

Re: Basic model management

When what is checked?

 

I'm still wondering where the switch is for Reference and Construction. I have run into the construction switch before and thought...that could be useful, but now I cant find it.

 

I'm out for the next week, I will check this thread out the following monday.

Re: Basic model management

[ Edited ]

"Higher Level" has been there at least on ST6. So what changed exaclty?

Though 12gage should also say no to higher level if he's using the part in an assembly and doesn't want it to appear at higher levels.

Bruce Shand
ST9 MP8 - Insight - Win10 - K4200

Re: Basic model management

Apparently the name change to "higher level" was done previously. The key thing that changed in ST7 was performance. In the past, if you were at a higher level and down below someone had an assembly marked "no" for higher level, it would not be displayed, but you would still pay some penalty in chasing down the files and some memory footprint. 

 

In ST7, the "higher level" switch basically cuts the tree completely, so higher level documents do not even know the lower lever private reference exists. This primarily matters to those doing very large assemblies (and to them it matters A LOT because the performance improvement can be remarkable).

Dan Staples
Director, Solid Edge Product Development