I think this should be a first grade question but when I
sketch a shape (a square for example) and extrude with draft and
thin feature, only one surface has draft. I also took the sketch
and did an off-set and extruded with draft and the same problem.
I would like to make a plastic part with draft and keep the material thickness the same without a secondary cut extrude or adding draft after.
Sounds simple but what am I missing?
Thanks, Kevin
SW2008 (I will add a signature line some day....)
I would like to make a plastic part with draft and keep the material thickness the same without a secondary cut extrude or adding draft after.
Sounds simple but what am I missing?
Thanks, Kevin
SW2008 (I will add a signature line some day....)
Short answer: it works right for me. why do you think you only get draft on one side? You can't even make it do that if you want to.
Oh, I might be seeing what you are getting at. You want to extrude a thin feature and keep the faces parallel, but draft them both from opposite directions.
You can't do that. You have to extrude a solid and shell as suggested or make two draft features.
One way you could do it would be to extrude a surface with draft instead of a solid, and then thicken the surface. That would work and give you parallel drafted faces, but the end faces would be perpendicular to the drafted faces rather than perpendicular to the direction of pull. Plus, I'll bet you're looking for something simple.
Personally, I prefer draft as a separate feature. Putting some draft in extrude features and other draft in separate features makes it tough to go back later and ediit the draft, because you can never find it.
I draft my extrudes within the extrude feature. I am trying to think of an example where it would be hard to find the draft to change it. If I have an extruded feature that is drafted, I just right click the feature, and edit feature. The draft is right there. Less features in the tree too.
The only time I use draft as as seperate feature is when it can't be included in the extrude, such as when one wall would have different draft.
I'm not trying to argue your parctice as much as trying to understand and learn. I'm sure I draft my features this way because that's the first place I saw to do it as I started learning solidworks. I don't want to fall into habits simply because I lerned it that way. I want to be as efficient as possible.
Paul
Also when you need to put fillets on a part before draft and can't do it as part of an extrude. That would be fairly rare, the first situation happens very frequently.
If you have a part with a couple dozen draft features and an equal amount of draft created in extrude features, it can be easy to lose track of where a particular face is drafted.
Of course it doesn't matter much , because the last draft feature to touch a face wins. You can apply as many draft features as you want to the same face, and it will only be drafted by the last feature. Still, you get negative style points for double drafting faces.
Great ideas from all. When I'm working on a model, add a feature and shell or add draft after, the shell or draft can shell or draft more than I want. I think if I do an extrude with thin feature of say .120" thick, my extrude will always be .120" thick without adding a second cut extrude, linking sketches and dimensions so when the extrude is edited, the secondary cut updates also. Maybe in SW 2010??
I think I know what you're saying, but I think you are taking the wrong approach. Before I get started, I want to remind you that this is my opinion, but I am pretty sure it's accurate for a general approach.
It sounds like you are trying to take too much control a little bit to early in the design process. By that I mean you shouldn't be too concerned about your wall thickness until you have most of the major design components in place. Typically, for me, I procede like this...
1. Create my main extrude (not thin walled)
2. Add any other basic extrudes
3. Add drafts
4. Add a fillets
5. Shell
6. Add finer details and holes
7. Add mounting bosses, strength ribs, etc.
Steps 1-4 are most of the job. You try to define the basic shape of the part here. You don't need to worry about the inside at this point. Pretend it's not a hollow part.
Step 5 is where you gain control over thickness
Step 6 is when you would add features that you wouldn't want to shell. Typically these features would be through holes, ribs/lips, engraving, etc.
Step 7 would take place once the part is complete. Just add features you need to assemble the part, strengthen it, etc. Typically this all happens on the inside of the "shell"
This is by no means a definitave approach. Things are different all of the time. I just feel that you are worrying about the inside of the part well before you need to. The shell command is powerful, and you should take advantage of it.
I hope this helps. If I've told you thing you already know, just ignore my post.
Paul