when i am going to extrude cut there is lots of contours in the same sketch thats why my lappy gets slow and it takes a lot of time for extrude cut.
What i should to do extrude cut in minimum time and with minimum commands.
If you select the closed contours of a single sketch, you'll be able to do that BUT that's a lot of closed contours. Good luck!
Can you detect a pattern, maybe that will help...
how all closed contour is to be selected is there any option in extrude cut?
Here's a sketch on a face.
I'm selecting the closed areas that I want to cut. Note the selected contours in the selection window at the bottom of the Cut-Extrude
This sis what I get
Does that explain it?
Thanks steve for your information but its a single cut i am talking about multiple closed contour. I am totally fed up to do one by one extrude of closed contour & it is taking a lots of time.
Ok, it looks like you did a pattern to create that. Why couldn't you do this with some patterns? It looks like, in your original picture, that patterning could solve some of it but you're going to have to understand, this does take time bth creating the sketches and doing the cuts
Here, this was done with the 3 smaller circles and then patterned.
can you show me the feature manager tree steve? How you pattern it?
Does that help?
Thanks Steve it helps me but on inside periphery the circle is not cut its side portion is extruded cut then how that is to be patterned.
I don't understand your question Awaish?
Your sketch lines overlap, you need to add a space, can be really really small, but there needs to be a space between the holes and the ring...
I believe Steve was saying to remove the sketch pattern, and create a feature pattern.
In your sketch, you have 6 different patterns -
Create 6 new sketches, each with a single circle, to make the cut, and then pattern each of the cuts individually.
It will create a lot more in your FM tree (as you see in Steve's example), but it will perform much better.
When in doubt, simplify your sketches . . .
Todd Blacksher wrote: I believe Steve was saying to remove the sketch pattern, and create a feature pattern.In your sketch, you have 6 different patterns -Create 6 new sketches, each with a single circle, to make the cut, and then pattern each of the cuts individually.It will create a lot more in your FM tree (as you see in Steve's example), but it will perform much better.When in doubt, simplify your sketches . . .
Todd Blacksher wrote:
That's excellent advice. And I agree that it's almost always better to create a feature with a simple sketch and then pattern the feature (or body) than to have sketch patterns.
The other nice perk about creating feature patterns is that you can create a configuration to suppress them all, so you can work with an extremely "lightweight" model, and only turn on all the detail when it is truly necessary.
1... and feature patterns are much easier to edit.
2...and you can easily configure the distance and/or number of instances for feature patterns if needed.
Glenn, that's sort of where I was going. The pattern, if one can be found, are usually faster and easier to work with.
Looks like Glenn and I were picking up what you were putting down from the get go . . .
(because it was really good advice)
I think doing something like Awaish is trying to do will no doubt take computer time and there's really no "Easy" button.
I'm now wondering, if this a piece of sheet metal, could all the patterning be done in the flat?
Maybe if I have some time around lunch, I'll give it a try...
Thanks all of you for your valuable knowledge. As Todd said you have to sketch six different circle & make them patterned individually , I think the feature manager tree is going too high and i try it but it takes a lot of time from both the way.
Hiii Steve i think you try it, would you find something new way to solve that problems
There is no easy button here, you're going to have to do some work and when you're finished, put the features in folders so your tree doesn't look so high (as you say).
Also, while I type, I'm thinking there may be yet another method. I wonder if we've thought of using a sheet metal forming tool to do those circular patterns?
I don't think making a pattern is a proper solution. This is an issue I'm having as well except I need to cut extrude outline of text brought in via a dxf from an illustrator file. I need to individually select each closed contoured letter which takes a large amount of time. This doesn't only apply to letters, it could be random shapes which aren't in a pattern, dxf files of patterns brought in from other sources, etc... There's so many situations where patterning is not a viable solution.
Surely there's a way where we can just select the sketch and Solidworks automatically picks all the contours to be cut-extrude / extrude instead of us having to select them all individually. I'm sure Solidworks had this feature in the past (or maybe it was another piece of software I was using), but not sure why it's not doing this any more.
If the contours are not connected and they're closed, then it would pick all of them
I tested this out and you are right Deepak, if the contours are not connected and closed, it would pick all of them. If there is a connected closed contour like the one below, it doesn't work. With the text I had, it had connected closed contours from the illustrator file which is why Solidworks didn't automatically pick up all the closed contours. I should delete the connecting lines next time, save me a lot of time down the line. Thanks Deepak!
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