How do I keep my sketches out of the features in the Feature Manager?

[bnemec]

In Solid Edge I learned to sketch out the important stuff in sketches on the base planes (and sometimes sketch on a ref plane that was defined (offset) by an earlier sketch. So I would have most of the important features (not model features, rather physical object features) defined in those various sketches on various planes before making the sketch that drives the starting solid body. That way I could move holes and reshape the cutouts in one place in those earlier sketches and most of the time the features would update nicely. In Solid Edge (and Inventor) those sketches were not absorbed by the feature that used them. It's really making this process clumsy. I understand I can have those sketches then include geometry in later sketches that are consumed by the feature, but that requires more fixing of stuff and is just as clumsy.

I'm beginning to think that my modeling method is junk.

Here's and example, the last sketch is for the base flange, it is driven by the previous two sketches.

Now the sketches are absorbed by the features which puts the sketches in backwards order and in more complicated part hides them all over the tree. It used to be so clean when the sketches stayed at the top. I make use of history based modeling, I used the entire feature tree when working on a part's design. People that just keep adding tabs and flanges then cut holes then cut away then add more then cut that off then add edge flange then unbend the flange to cut a hole then bend the flange..... UGHH, that's what ST is for! I do my best to keep a clear concise feature tree so the model can be precisely controlled in a predictable manner.

[mike miller]

Solidworks has taken the traditional, disciplined workflow from Pro/E and made it "easier" to use and therefore much more fast and loose. In fact, they've taken it to the point where the more stable methods are almost impossible to use (think of what they've done to mate folders, automatic mate flipping, and sketch consumption; to name just a few). That is exactly what you are seeing here.

All this is a long preamble to say: you're doing it wrong for SWX, at least IMHO. I would extrude the entire profile symmetrically as a Thin Base-flange feature, lop the corners off with a Cut-Extrude, use Hole Wizard to put the holes in, and fillet the corners. You can still relate one sketch to another after it has been consumed, you just have to unhide it. Or, you could sketch the entire "top" of the part as a Base-Flange, add an edge flange, use Hole Wizard for the holes (or just add circles in the sketches ) and fillet.

Alternatively, you could create a sketch part as a master and bring it in with Insert Part (basically SSP lite), but there's really no point if you have no external references.

[bnemec]

Solidworks has taken the traditional, disciplined workflow from Pro/E and made it "easier" to use and therefore much more fast and loose. In fact, they've taken it to the point where the more stable methods are almost impossible to use (think of what they've done to mate folders, automatic mate flipping, and sketch consumption; to name just a few). That is exactly what you are seeing here.

All this is a long preamble to say: you're doing it wrong for SWX, at least IMHO. I would extrude the entire profile symmetrically as a Thin Base-flange feature, lop the corners off with a Cut-Extrude, use Hole Wizard to put the holes in, and fillet the corners. You can still relate one sketch to another after it has been consumed, you just have to unhide it. Or, you could sketch the entire "top" of the part as a Base-Flange, add an edge flange, use Hole Wizard for the holes (or just add circles in the sketches ) and fillet.

Alternatively, you could create a sketch part as a master and bring it in with Insert Part (basically SSP lite), but there's really no point if you have no external references.

Thank you for the reply. The whole point of making the sketches pretty much backwards, is that the hole define the size of the blank. If I move the holes there's no way to have the blank update to accommodate the move. In this case it's a mute point as the filter head is what it is. But in the case of designing a new suspension the top and bottom housings and links all change a bunch and having to update the base tab profile after moving the holes every time is a pain. I like having one or two, maybe three sketches contain the elements that defined the overall of the part. I could still have those sketches as "Master Sketches" just put them in this part (as you said there's no external refs) and Convert Entities (Include Geometry in SE) but that makes a bit more work to keep updated.

Maybe not so terrible I guess as sometimes I would use include geometry method so that I could delete segments in the master sketch without killing the feature. The sketch that had "Converted Entities" would need fixed by reattaching those sketch elements with relations, but the feature that was using those converted entities was still ok, which meant less chance of new internal IDs which kill Mates and Annotations on prints.

[bnemec]

Maybe not so terrible I guess as sometimes I would use include geometry method so that I could delete segments in the master sketch without killing the feature. The sketch that had "Converted Entities" would need fixed by reattaching those sketch elements with relations, but the feature that was using those converted entities was still ok, which meant less chance of new internal IDs which kill Mates and Annotations on prints.

This is nice, I don't recall being aware of SE having this feature of "Replace Entity"

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[JSculley]

Right click the top of the feature tree, select Tree Display and select Flat View.

[CarrieIves]

While it may be somewhat double the work, you could create the controlling sketches at the top of your tree, and then for each feature, make a new sketch that uses edges from the controlling sketches.

[Frederick_Law]

You are using Master Sketch with the Master in the part.
Put the sketch in a part file and insert it in a new part.
It'll always be on the top.

[bnemec]

You are using Master Sketch with the Master in the part.
Put the sketch in a part file and insert it in a new part.
It'll always be on the top.

um, that's a file management nightmare, so every part file that I would want to model this way would need another part file just for it's master sketch. I see no way that we safely use any top-down modeling methods. I guarantee you before that files gets to rev 5 someone will try to edit the part, won't know they need to check out the other file and think they've made changes, then save and check in then the next person opens it with some mix of the master sketch in another file and the edits made without the extra file. Then the pdf and dxf will be published during the Release transition and be junk, then it'll be a no-rev change...

The way the "Master file" method keeps getting promoted I gotta be missing something or have some huge mental block.

[Frederick_Law]

All methods has pro and con.
You need to develop your own workflow.
And if the Master only used in one part, don't do insert.

There is nothing wrong changing part without changing Master.

[mike miller]

um, that's a file management nightmare, so every part file that I would want to model this way would need another part file just for it's master sketch. I see no way that we safely use any top-down modeling methods. I guarantee you before that files gets to rev 5 someone will try to edit the part, won't know they need to check out the other file and think they've made changes, then save and check in then the next person opens it with some mix of the master sketch in another file and the edits made without the extra file. Then the pdf and dxf will be published during the Release transition and be junk, then it'll be a no-rev change...

The way the "Master file" method keeps getting promoted I gotta be missing something or have some huge mental block.

"Master" method is not for everything. (Hey BTW, isn't it r@cist to use that word?)

What I would do is model it with the "Top" of the part for a Base-Flange and put sketch points in to define the hole location. Then, show the sketch and pick the points up with the Hole Wizard.

[bnemec]

"Master" method is not for everything. (Hey BTW, isn't it r@cist to use that word?)

What I would do is model it with the "Top" of the part for a Base-Flange and put sketch points in to define the hole location. Then, show the sketch and pick the points up with the Hole Wizard.

Well, much of the time we are making Sheetmetal parts, so I haven't seen a need for Hole Wizard, just use extrude cut with normal cut selected. I could put the hole profile on a later sketch, but it's the edge of the hole/cut that drives the outer shape of the base tab/flange so I need the cut profile back in the beginning as that drives the sketch of the base feature.

That's not a hard and fast rule, but in pure form that's the point of putting the cutout profiles in sketches that exist before the sketch that makes the base tab/flange.

[jcapriotti]

@bnemec We do the same to drive design intent. What I do is created the layout sketches like you did, but when it comes time to create a feature, start a new sketch, select the layout sketch and convert entities which copies the everything over linked. Or sometimes I just convert certain items.

For the holes I just add sketch points and snap them to the layout sketch. I prefer to use the hole wizard when possible so the layout just has points, but you could draw the circles and had the size there as well.

[HerrTick]

It took me a bit to figure out why the OP has a problem, as I am so habituated to doing this in a SW-friendly way (which I actually started doing in Pro/E).

IN my "CAD orthodoxy", layout sketches are for layout. They are never used for directly making solid or surface features. They are only used for reference geometry or constraining downstream sketches.

I don't worry about any "extra" work this generates. The added work is minimal to those whose skills are not. The additional layer of connection gives the model a measure of robustitude that saves time and headaches when later, unforeseeable changes impact the model.

[Glenn Schroeder]

It took me a bit to figure out why the OP has a problem, as I am so habituated to doing this in a SW-friendly way (which I actually started doing in Pro/E).

IN my "CAD orthodoxy", layout sketches are for layout. They are never used for directly making solid or surface features. They are only used for reference geometry or constraining downstream sketches.

I don't worry about any "extra" work this generates. The added work is minimal to those whose skills are not. The additional layer of connection gives the model a measure of robustitude that saves time and headaches when later, unforeseeable changes impact the model.

Makes sense to me. I'm the weirdo who always uses a separate sketch to drive Hole Wizard features. By the way, I learned a new word today. Thanks.

[bnemec]

It took me a bit to figure out why the OP has a problem, as I am so habituated to doing this in a SW-friendly way (which I actually started doing in Pro/E).

IN my "CAD orthodoxy", layout sketches are for layout. They are never used for directly making solid or surface features. They are only used for reference geometry or constraining downstream sketches.

I don't worry about any "extra" work this generates. The added work is minimal to those whose skills are not. The additional layer of connection gives the model a measure of robustitude that saves time and headaches when later, unforeseeable changes impact the model.

It sounds like you explained the issue, I was not used to always needing the extra sketch for the feature, just use the sketch that already existed. Solid Edge has "Include Geometry" which is like "Convert Entities" in SW and I used it a lot to get edges from surfaces and bodies but not always to get sketch elements from other sketches. Pretty much just when I wanted the extra layer of robustitude you mention. This worked well when I pretty much expected the master sketch element to be deleted at some point. That just breaks the sketch element instead of the feature and all the down stream features so simpler fix.