sheetmetal flat in the drawing...

[design-engine]

There are several ways to create a flat and drop that view into a Creo drawing. Family table is one. Is there a new way with Creo?

Simplified reps in a part?

What is your common methodology?

 

[magnusod]

I believe that there's not a new way other than a shortcut to create a family table instance from the interface. We use Simp Rep which needs an Unbend followed by a Bend back feature which is supressed in the Flat Simp Rep. After that a Combined state is created so that the flat state can be shown on a drawing. We use a mapkey to create the Simp Rep and the Combined Rep on the modeling side.
Here's a thread on PTC Community which might indicate that we could see an improvement in Creo 3.0 or 4.0 PTC Community: Creo 2.0 - Q: Is the flat state easier to create in PTC Creo than in Wildfire 5?

 

[Coosa]

I use the create flat state option to create a family table, but you now have to have a config option to allow flat states for some reason (enable_flat)state).

 

[srieger]

I believe that there's not a new way other than a shortcut to create a family table instance from the interface. We use Simp Rep which needs an Unbend followed by a Bend back feature which is supressed in the Flat Simp Rep. After that a Combined state is created so that the flat state can be shown on a drawing. We use a mapkey to create the Simp Rep and the Combined Rep on the modeling side.

This is a pretty odd way to do it. In Creo, Simply select "Flat Pattern". After the flat pattern feature is created, in the same dropdown menu there is pick that will now be enable called "Create Instance". Select this and change the fixed plane reference is required, update the name if required. Accept then suppress the flat pattern feature in the generic.

In the drawing, simply place the views for the generic, add the flat pattern model to the drawing, add the view for the flat pattern. Very simple, no simplified reps required, no combined state required. No mapkey really required.

 

[magnusod]

It might seem odd but it's getting more common. Getting rid of the instance makes life easier in PDMLink. The Combined Views can also be displayed so that you can toggle between bend part and flat state with the tabs below graphic area.
The mapkey is simple and when you add a view on the drawing you can choose directly if you want to add the bent or the flat state. No need to add an instance to the drawing.

As I wrote in the PTC Community thread I hope they will add a flat state by default so that you can toggle between flat and bent state. I believe most other CAD programs have that functionality. It shouldn't be hard as they added the preview flat window in Creo. I prefer to have the family table for variances. If you create variances and then want to have flat states you either have to add that feature in the table or create nested family tables which can be a bit tricky.

 

[jdurston007]

I have always just used the Flat Pattern feature and put it into a family table. It hasn't given my any problems when I worked at places that had Pro/INTRALINK. We are not on Windchill yet; so, I have yet to experience the problems people are having with family tables. (People used to complain about it on Pro/I and Pro/PDM as well..) I have used Unbend / Bend Back if I want to get a feature that I have to create in the flat, but then I might create a Flat Pattern feature anyway. It's nice because it's always the last feature. This makes it nice for mapkeys.

Set Up / Flat State (BTW) is just a fancy way to create an Unbend with family table. It's like a PTC built in mapkey.

There was some talk about eliminating one or the other.

The simplified rep method is intriguing. I may try it one day, but I don't have a compelling reason to use it right now. I have seen it before on the forums.

You have to be careful about how you use Unbend / Bend Back, because you can create a mess with multiple UB/BB pairs. I would keep these pretty late in the model tree order as well in case of developing any unwanted parent-child relationships.

I evaluated Solid Edge for my company (2 jobs ago) and it's sheet metal package is pretty nice. The flat pattern is just a view option. There is no need to create a feature for it. This was almost 10 years ago. It would be nice if PTC would come up with something similar (assuming that the geometry could be flattened.) Both this and family table functionality needs a serious revision.

 

[srieger]

I use family tables extensively with PDMLink. Including for flat patterns. They work fine as long as you follow the rules. Nested family tables are never a good idea, particularly with PDMLink. They can be done but it can be troublesome.

The problem with creating a flat pattern that is just a View or even a simplified rep kind of depends on how you use it. For me, many times I have to add features to the flat that are only in the flat to help with gaging the part. This is much better to do in my opinion as a family table. It also allows a much easier method for creating many variants and still using the same features for the flat.

To say people are moving away from using the family table method is a bit far fetched. I think both methods have their place.

I guess it all depends on what works best for you.

 

[design-engine]

thanks everyone.

 

[design-engine]

Many companies don't want to for various reasons to utilize family tables w/ windchill. With his said we are teaching vagarious workflows alternate to family tables. Family tables in the part aids in the flatten state in the drawing. From a windchill perspective an inheritance feature method may be the best way for a sheetmetal part to be used in the assembly.