I have tried to jump on the Synchronous Sheet Metal bus a few times, but it seems every time I do, I am quickly kicked to the curb. So, I thought I'd lay out the problems that stonewall me and either get some suggestions from smarter people than I, or find someone to commiserate with. It took me two years or so to figure out the Shift+Click on the sync steering wheel to change the active plane, so I don't hold high hopes for my ability to figure this all out myself.
Below I've made a generic sheet metal part that has a lot of the features I might deal with on a daily basis. Some square edges, some profile areas, some slots, a weld prep bevel on one edge, and small radii on all of the outer corners. I'll use this file to experiment with some typical edits and see how I can handle them in Synchronous vs. Ordered. Most of the sheet metal details I create go into very tight tolerance sheet metal assemblies, and as such I am constantly changing/tipping trims, profiles, etc to accommodate for shrinkage. Actually creating the initial geometry probably ends up as 10% of my time investment in a detail- the rest of the time is spent editing this detail as it goes through prototype revisions. So, this sounds like a perfect case for sync, right? I make thousands of edits per week on hundreds of details- currently all in ordered mode. This is why 3/4 of my started threads are sketch pet peeves- a wasted click or a screwy tab order costs me a lot of time when it's x1000 every week.
The first thing I run into before I even do any editing is that I must create the bevel Cutout on this example part in Ordered mode. Why? Is this a purely technical limitation? It's not like SE needs to know the perfectly flattenable sheet metal shape, because my flat pattern DXF still exports a bunch of lines showing the cut extents of the bevel. This is another pet peeve. I want to take this file and laser it, and then machine the edge. Why do I have to either sit there and edit the DXF to remove these bevel lines, or make TWO linked files, one with the bevel and one without, to simply produce a flat pattern that represents that stage of the manufacturing process? I have to imagine there is a better way- perhaps the flat pattern dialog allows you to click on features to exclude them from the flatten and export?
Moving on to the common edits-
Below in the first picture, I've highlighted a chain of surfaces I'd like to offset. In the second picture, I've drawn a rough sketch of where I'd like them to end up as an end result.
Unless I am missing something, there is no way to offset these elements in this manner (each surface normal to its original vector) all at once by using the steering wheel, and offsetting them individually is not desired. This leaves two options.
1. Draw a sketch of the desired offset, similar to the picture above, and close the ends and add the material of the now enclosed sketch using the steering wheel.
2. Go into the surfacing tab, offset these surfaces, and use the Replace Face command. This, however, requires deleting the rounds on the ends of the profile chain, and/or extending the offset surfaces, to allow the Replace Face command to work.
BOTH of these methods still break any assembly relationships that might have existed to the original surfaces in that profile chain, and BOTH of these methods have the possibility of breaking the Cutout 1 bevel feature if it was not foolproofed for this specific edit when it was made. So, for this type of edit, we see no benefit to Synchronous sheet metal for speed of the edit, and we also still have to deal with the same number of possible broken features/relationships/links that we would have if we had done a 100% Ordered model.
Here, Synchronous sheet metal is much better at handling the edit than an ordered approach. Weld shrinkage may dictate that I have to tip a side by as little as 0.003". Below is a video showing me making this edit in Synchronous, which involves offsetting the surface, then rotating the edge to the corner of the offset surface. In ordered, this would require editing the base sketch, rotating the line, redoing the trims and end radii, and then finishing the feature and hoping you've retained all the original geometry so it doesn't break features down the line. Depending on if the move is square to the sketch plane, you could try to use the Stretch command in Ordered sketch, but this command has gone unloved for a long time and breaks fillet features, behaves badly when you try to zoom while in the command, and does generally wonky stuff that people steer clear of when they actually care about the shape of the part they're trying to make.
I'll be posting more musings/comparisons here soon, and creating another example to put my toe in the water on Sync vs Ordered simple bends.
Solved! Go to Solution.
I think power of Solid Edge is in the mixed mode. Yes, synch sheetmetal has some limitations (probable, developer team works on them).
Here is a video what can be useful for you:
in the first part of video you can see what I suggest doing flatten parts state. If you are in flat pattern you can edit the model (add or remove material, resize hole, etc). Family of part without populate (all model state would be in one part/model) should be nice for this.
In the second part you can see that I'm doing offset on the model in ordered mode! May be this is the simplest way!
Tipping an edge-
Just an initial comment / question.....do you do this "Edge Tipping" for the main model and use it in the assembly? I typically want the assembly, and it's component files to be in the finished condition. [I tend to use "alternate condition" models for further processing instruction]
When I've needed similar corrective mods, I'll do them in the "Flat Pattern" state...but the lack of tools that operate in that mode, while it's better than it has been, is still sorely lacking. [Break edge & Hole, iare two such missing tools I like to use there]
Sorry, I'm really slammed at the moment, even with my second user we just added....will try to take a look at it after work.
Design Manager Streetscape Ltd
Solid Edge ST10 [MP7] Classic [x2 seats]
Windows 10 - Quadro P2000
Thank you for the insight, Imics, Sean.
Sean, I do sometimes split the assemblies. It is difficult to decide when to do so. Our parts are 100% welded and are fairly complex and small, so there is a massive amount of warping and shrinking. Sometimes, by the end of ten or so development revisions, I have sheet metal details that are 'tipped' 0.100" or more from a perfect-world CAD number! So, how do you maintain two assemblies, one that represents the end result, one that represents real-life manufacturing trim requirements, both of which are feature complete, across an assembly that has 30-60 such details all getting constantly revised? I've built macros to do as much as is possible, which I suppose is an unfair hit against my approach to synchronous, because I don't have the same toolset to help reduce my edit times and general overhead.
So, how do you maintain two assemblies, one that represents the end result, one that represents real-life manufacturing trim requirements, both of which are feature complete, across an assembly that has 30-60 such details all getting constantly revised?
I don't make another assembly [normally] as such, just the alternate part file, by way of a "Part Copy" then adding the upstream "production manipulation" features to that copy of the parent model......but for the most part, I'd try to do this strictly inside the "flat pattern" [renaming for meaningful feature names] of the PSM, and make detailing in the DFT, if need be, for what, where & why.
I think Imi covered this example part of pretty well....many of his videos make me realise how much I need to get some more training....and I would be OK [bank manager may disagree] with going to Hungary to get it.
Design Manager Streetscape Ltd
Solid Edge ST10 [MP7] Classic [x2 seats]
Windows 10 - Quadro P2000
I'm going through the same thing, trying to move to Sync from ordered, but I'm thinking about completely different problems.
My sheet metal includes cross breaks and dimples. Even if I do a sheet in Sync, I must ordered features to model the part.
For many of my parts, I need to separate the flat pattern size and location of the bend lines. This can't be done is Sync. To be more clear about this one, Say I'm making a 10 x 10 x 10 box. The Lid will be made from an 11 x 11 piece of sheet metal. Exactly where the bends go and what notches are used depend on the tank design.
Imacs just did me a huge favor by posting a sync perametric box Method. Much much better than using planes in ordered. I plan to use Sync for all my size defining parts, then use odered for the rest that use the Sync part to set the dimensions.
There are more things I would like to add, but out of time for right now.
Just so we're clear -- there is nothing particularly "wrong" with mixing and doing the base shapes in Sync and the other stuff in Ordered. This is one very powerful aspect of the system and why we built the hybrid tree from ST3 onwards...
One detail I have been pondering since I started is attaching a hole to a part that will be added. Say I add a coupling into a piece of sheet metal. I would like the hole for the coupling to be part of the coupling file. This way, if the fitting is right, so is the cutout for the fitting.
I have yet to figure out how to have a hole as the first item in a tree. The reason I bring this up here is I'm wondering if I can take advantage of the relations between sync and ordered to trick a hole into being the first item. If I trim the hole afterwards, the part being added also gets trimmed. at least if I set the cut to cut everything. If I set up the cut to be specific to the sheet, then I don't see attaching a hole to a coupling as practical.
Right now im using sketches in ordered to place holes, and then place the fitting into the hole. I must keep track of what fitting will fo there and cut the correct hole for the fitting. Mmoving to sync I will end up with an XY dimension and Diamiter for each hole.
I have no problem mixing sync and ordered features when it benefits me, but why am I being forced out of synchronous for this? Is it a technical limitation or is it something that just hasn't been added in to Sync sheet metal yet?
Nothing forces one to use sync for anything, however, I'm trying to use Sync for sheet metal to accomplish the perametric box without using planes. Dimensions controlling the outside of a sheet metal box work great in sync. My problem is that I can't make the part at all in sync that I can in ordered.