Re-deriving sketch?

It's because of this that I rarely use derived sketches in-context. They just can't be repaired. You'll have to insert new derived sketches, and rebuild the parts on the new sketches. You shouldn't have to rebuild all these parts entirely though. Insert the new derived sketches, and remake the initial features (unless the derived sketches were not consumed in features). After that, use the parent/child tools to track down and transefer all the relationships from the old derived sketches to the new.

This might better be used as an opportunity to use something other than derived sketches. What that would be probably depends in how complex they are and how you were using them.

HTH

Daniel,

If you really used in-context references rather than the Derived Sketch function, you may be able to reattach the references by clicking a line, click and drag the red dot to an appropriate entity. As Dale says, though, you're hosed if you used Derived Sketches.

A way around this would be to leave a copy of the part in the original assembly, but hide it. You can't convert a regular part to an envelope, which would be ideal. Leaving it hidden isn't ideal, but it keeps your references from exploding.

Anyway, good luck,

Matt

Am 07.03.2006, 15:30 Uhr, schrieb matt :

OK, I'm hosed then.

Good tip.

What it boils down to is that it pays off to spend an extra hour on really thinking how all the interdependencies in a large project are.

My project uses two basic contours (the inner and outer part of sort of a bayonet mount) that re-appear in various parts that don't have a hell of a lot to do with each other but are all part of the same assembly tree. Not so much because they really are going to be assembled in that manner, but to see how it all moves together.

If I'd start over I'd probably draw a couple of reference sketches at assembly level and derive the part sketches from those. Is this a good approach in general, or how would you guys do it?

Thanks,

--Daniel

Daniel,

I use derived sketches all of the time and rarely have problems with it. It is about 10X faster than any other in-context features, and really makes your assemblies fly.

Now back to your problem. Well, it really isn't a problem.... Huh?!?! This is going to blow a lot of peoples minds, especially the people that don't like derived sketches.

Ok, even though the derived sketch was actually derived within another assembly, as long as your master part "A" is open and resolved in the new assembly along with part "B" (which it sounds like it is), then the part "B" derived sketch WILL update properly when the master part "A" sketch changes. At least that's the way it used to work. Yes, you will get the "?" in the new assembly. I just ignore it.

I used to do this a lot and never had any problems. I know it is "technically" not the best practice. But if it works with no problems, HEY......

I have not tried this in SW2006 so I can't say for sure that it still works. But logically, I don't see why it shouldn't.

You just reminded me of a potential workaround. If you have 2006, you can use saved sketch blocks instead of derived sketches. Sketch block references are repairable, and you can get at them without loading the assembly. So, you would need to create a block of your orignial sketches, save the files and link them to the new block files. In the derived sketches, underive them, then insert the blocks. You'll probably have some dangling or tangled references, but I think it'll be a quicker repair job than re-creating the derived sketches.

Seth, you don't have trouble with them? Since at least 2003, I've had derived sketches in assembly files that won't update unless you open them (and they're not even broken).

Knock on wood, I have never run into any significant problems! As far as I'm concerned, derived sketches are "Da Bomb"! Derived sketches are my MOST USED in-context feature when designing molds. Every part in my molds (except library parts) has AT LEAST 1 derived sketch, usually 3, and sometimes as many as 6. There are a few other in-context features like base parts and a cavity feature or two. But derived sketches is what basically builds my mold assemblies. And, the biggest advantage is that they don't take a lot of horsepower from your computer like most in-context features do.

If you are having trouble with them, we must be doing something different, or have an option set different or something.

I think I might use them more if they could be easily repaired. I can see how they would require less horsepower from the PC, since sketches are copied complete instead of in pieces, sort of without having to be solved.

Where I have trouble with them functionaly may not be a problem specifically with derived sketches. I have a commonly copied subassembly with some derived sketches at the end of the tree (in the assembly doc). These are the ones that only update when I open them. Lately though, I've been noticing some other odd rebuild behavior down there. So, it may not be derived sketches' fault. Do you ever use derived sketches below the mate group?

I am not sure exactly what you are asking.

I don't know if this will make any sense due to different industries that we are in. But, in a nutshell, here is the way I use the derived sketches. I'll try not to be too detailed. But that's difficult for me. :)

1. plastic part model put into what I call a "sketch assembly"
2. create assembly sketches (3 minimum). only sketch on assembly planes. these sketches are to define many things, molding-insert sizes/shapes, screw locations, ejector locations, etc. the rule of thumb is, if it will effect

1. insert 2 parts that will be used as a-side and b-side base-parts. it is important that ALL parts be inserted directly on the origin, or mated plane to plane with all of the default assembly planes
2. use the assembly sketches and cavity features to create the base-parts. base-parts is the one instance that I may or may not derive the sketches. if the in-context stuff is simple enough, I may simply reference the sketches directly in the assembly
3. you should now have a "sketch assembly" that contains the plastic part model, sketches to define the molding-inserts, an a-side base-part, and a b-side base-part
4. insert this "sketch assembly" into the "final assembly" as a sub-assembly. hide it if necessary
5. insert new parts into this "final assembly" that will be the molding-inserts parts. here again, directly on the origin or mated plane to plane
6. in the parts, insert the base-parts as needed (a-side base-part into a-side inserts, etc.)
7. back to the "final assembly", derive the sketches from the "sketch assembly" into each of the molding-insert parts. in each of the molding-insert parts, you should now have a solid body inserted from the base parts, and all of the derived sketches.
8. you can do all of the referencing for splitting into molding-inserts, screw holes, heals, ejector holes, etc. directly from the derived sketches within each part, not in the assembly. this is where it saves big-time on pc power.
9. if you see something that you missed, or don't have just right, simply go back to the "sketch assembly" to make the changes, and it will propagate down to all of the molding-insert parts.

Hope you can make heads or tails of this. This is very basic. There is a little more to it. But it should be good enough to get an idea of how I am using them.

One of the issues with Top Down design is that Yesterday's top is today's middle or bottom.

"Seth Renigar" wrote in news:XDBPf.31265$ snipped-for-privacy@southeast.rr.com:

I followed all that pretty well. It sounds like you would never get near the particular usage I have trouble with. What I'm doing is tracing a part in the assembly (a quick convert entities, actually), then inserting a derived sketch of that into the same assembly to serve as an el cheapo alternate position view. All of this exists in the assembly, and is below the mate group in the FMT. This is usually a no-no for performace reasons, but it's the most expeditious way to accomplish this particular task.

Dale,

I don't know if this would make any difference or not, but why not create your traced sketch in the part, then derive that into the assembly. It may not make a bit of difference. But it just seems like the more logical way in my eyes.

"Seth Renigar" wrote in news:H%EPf.33021$ snipped-for-privacy@southeast.rr.com:

The reason why not is that I didn't think of it. I'll have to try that next time and see if it works any better. It just might work better, without having one time-based assembly item dependent on another. Thanks for the idea.

"Seth Renigar" wrote in >

Sounds a good method, provided the alternate view required is only of a single part.

Dale, why do you not wish to just add another instance of the part and mate it at an alternative position, or use another config to show it in more than one place?

John Harland

I occasionally do those things. Primarily, I use these as an alternate position without the overhead of an actual alternate position view. It's also a sort of schematic visual guide to how much room I need while I'm designing the assembly. This is separate from the configuration this subassembly has for the other position. One thing I get from this that I can't get from the other methods is a persistent set of construction lines depicting the path of motion. I could add that on drawing views, but this way, I simply make the sketch visible.

Hi guys,

thanks for all the help. This is a terrific newsgroup. I ended up solving my problems by creating a couple of reference sketches at the top assembly level and by deriving the relevant model sketches from those. For that of course I had to delete a lot of former model-level sketches and their associated features -- often followed by having to delete each and every feature of the model, ending up with a stack of unresolved sketchses. Sometimes I just hosed the entiere model and rebuilt it from scratch. This sounds worse than it was; in the end the reorganization of the project maybe cost me a couple of hours but will save many headaches in the long run.

Thanks again,

--Daniel

(During this process a new question popped up; I'll start a new thread for that).

A quick followup:

The new top-level assembly sketches are completely stand-alone and depend on nothing else. Why is it that they appear at the very bottom of the assembly tree (below mates) and cannot be moved to the top?

Thanks,

--Daniel

AFAIK, all "features" in assemblies go below the mate group. This should not pose any problems. It's just the way that they work.

This is a little flaky sometimes. Sometimes you get the pointer which means you can't, but it will work anyway if you try. Sometimes I don't drag high enough in the assembly tree, and I think that it's not letting me re-order the sketch. Sometimes it disallows the reorder for no discernable reason.