Treatment of Sketches Used for Modeling Functions

[kcoffield]

I've made a lot of progress learning Alibre but have several things that still seem to frustrate and cost me a lot of time. I'd sure like to figure out what it is I'm doing to avoid such. Here it goes.

1. I gathered that once a sketch is used for a modeling function, it is no longer available for any other function. For example loftfrom a sketch in one direction and extrude in the other is not allowed. Just confirming, Is that correct? I find myself having to duplicate sketches in the same/identical plane and position which seems like poor practice laying them on top of one another.
2. Once a sketch has been used for a solid such as extrusion, sweep, loft, etc, Is it forever associated with that function? Even if that feature is deleted? I ask, because say I use a sketch to extrude a solid, then I decide to remove/delete that extrusion and it is the last feature in the design tree. If I try to use that sketch for another extrusion or sweep or whatever, I get an error that says I am requesting the use of an item that has been deleted, but the skecthes status in the DE does not say that and displays without error in the DE. If I delete that sketch and create an identical new sketch for use, that solves the problem, but takes a lot time.
3. Somewhat similarly, if I use a a solid in a linear pattern, and I try to use that solid in any other way afterward, sometimes even just modifying the linear pattern or trying to mirror the linear pattern, I get an error that says the target is no longer available. So instead of mirroring an array of patterned solids, I have to create a new sketch in the mirrored position, create the solid, and pattern for multiples. Seems like similar to the above, once that solid got used in a pattern, it became forever unavailable for anything else. Is that normal?

So in both those examples above, it's like the sketch or solid is forever associated with the function which it was previously used andthereafter is rendered useless and must be recreated. Is that normal or just something I'm doing (or not doing)? I mIght be able to post an example if the questions are not clear.

Best,
Kelly

 

[DavidJ]

Not at main computer at the moment.

Item 1. You can use sketch as source for 'project to sketch' so can have multiple instances each used in separate feature. You can also copy/paste sketches. You can also use face of extrusion as one profile in a loft.

Item 2. Doesn't sound right, but can't check just now.

Item 3. Again, doesn't sound right, do you have example....?

 

[kcoffield]

Thanks for the quick reply.

I've used copy and paste to duplicate sketches but not the others. I'll experiment. Thanks for those suggestions.

I'll come back with examples of 2 & 3.

Best,
Kelly

 

[Ken226]

If you delete a feature, such as an extrusion, then the associated sketch becomes free for use in another function, and at another point within your workflow.

The order the features were created in can make a significant difference in the results. If you would like to use that sketch for a different feature, you can drag the sketch up or down the design explorer, to place it wherever you need within your sequence of features, then create another 3d feature at that point in the design tree.

Also, in the same way that the sketch can be moved up or down the design explorer. A 3d feature and it's associated sketch can be moved as well.

 

[Ex Machina]

I've made a lot of progress learning Alibre but have several things that still seem to frustrate and cost me a lot of time. I'd sure like to figure out what it is I'm doing to avoid such. Here it goes.

1. I gathered that once a sketch is used for a modeling function, it is no longer available for any other function. For example loftfrom a sketch in one direction and extrude in the other is not allowed. Just confirming, Is that correct? I find myself having to duplicate sketches in the same/identical plane and position which seems like poor practice laying them on top of one another.
2. Once a sketch has been used for a solid such as extrusion, sweep, loft, etc, Is it forever associated with that function? Even if that feature is deleted? I ask, because say I use a sketch to extrude a solid, then I decide to remove/delete that extrusion and it is the last feature in the design tree. If I try to use that sketch for another extrusion or sweep or whatever, I get an error that says I am requesting the use of an item that has been deleted, but the skecthes status in the DE does not say that and displays without error in the DE. If I delete that sketch and create an identical new sketch for use, that solves the problem, but takes a lot time.
3. Somewhat similarly, if I use a a solid in a linear pattern, and I try to use that solid in any other way afterward, sometimes even just modifying the linear pattern or trying to mirror the linear pattern, I get an error that says the target is no longer available. So instead of mirroring an array of patterned solids, I have to create a new sketch in the mirrored position, create the solid, and pattern for multiples. Seems like similar to the above, once that solid got used in a pattern, it became forever unavailable for anything else. Is that normal?

So in both those examples above, it's like the sketch or solid is forever associated with the function which it was previously used andthereafter is rendered useless and must be recreated. Is that normal or just something I'm doing (or not doing)? I mIght be able to post an example if the questions are not clear.

Best,
Kelly

Hey Kelly, here are my answer as far as I can understand your problems:

1. No you don't need to remake it. Just start a new sketch in the same plane, click Project to Sketch (top-left of the screen) and in the dialog box that opens select the sketch from the Design Explorer. Make sure to click maintain associativity.
See this video:

2. When you delete a feature the sketch is free to be re-used. I am not even sure why you would be getting an error. In fact, I do not remember getting that error in Alibre ever...

3. Nope, that is not normal either. Is this in a part or assembly file? Are you changing the order of features or rolling them back in anyway?

 

[DavidJ]

Item 3. After patterning a feature, the feature still exists - the pattern provides the extra copies. The two are separate but related features.

If for example you wanted to mirror the patterned features, you have to include the original (seed) feature AND the pattern in the Mirror command.

 

[Ex Machina]

Kelly, could you reproduce the error and get a screenshot. May e showing the DE as well. Might help

 

[kcoffield]

If for example you wanted to mirror the patterned features, you have to include the original (seed) feature AND the pattern in the Mirror command.

Ahhh, I think this could in part be the problem. I do recall seeing the option to include seed features but didn't understand what it meant and where I saw it. In the simple example attached, I don't see inclusion of seed features as an option in the mirror function. In fact, there are a couple of very fundamental things about linear patterns that confuse me.

In the attached example, I just created a simple 1" cube and use a linear pattern to replicate 3 cubes on 4" spacing. Then I mirror the pattern, but when I do, that first mirror only produces two cubes, and not the original (is that the seed?) cube. But if I perform a second mirror of the original cube it executes. Why is the second mirror necessary?

Further, if the original cube is not included in the pattern, why must I select 3 instances in the pattern instead of 2? Also, if I change the second direction from 1 instance to 0 instances then no pattern results, so I thought the original pattern is/was/must be included as one of the instances........but apparently not because it is not included when the pattern is mirrored. I experimentally concluded this and have been bumbling along with it but am not fully understanding the functionality of my pattern selections......maybe this is my problem?

If I try to edit that pattern after it is created, I can change number of instances and direction but cannot make it pattern in the second direction. Why?

This simple example does not replicate the "feature unavailable" issue. I'll have to come up with another example.

1. No you don't need to remake it. Just start a new sketch in the same plane,

I'll practice that before I come back with examples of the other sketch issues I mentioned.

Best,
Kelly

 

[DavidJ]

No need for second Mirror - just include the original (seed) and the pattern in the first Mirror.

 

[DavidJ]

The term 'instances' is chosen very carefully - it refers to total number of instances of the feature or part (which is usually what people want). Years ago the term 'repeats' was used (if I'm remembering correctly) but that didn't actually match the behaviour (as you say if it was repeats, you should specify one less than the total required.

 

[kcoffield]

No need for second Mirror - just include the original (seed) and the pattern in the first Mirror.

View attachment 39804

Ok, I get that for the mirror function. Seed geometry is just nomenclature not a selectable option in the mirror function.......just include the original seed geometry as part of the mirror.....but...

The term 'instances' is chosen very carefully - it refers to total number of instances of the feature or part (which is usually what people want). Years ago the term 'repeats' was used (if I'm remembering correctly) but that didn't actually match the behaviour (as you say if it was repeats, you should specify one less than the total required.

......so even though the original cube is one of the instances in the pattern command, it is not considered part of pattern when it is mirrored .......? That's what confuses me.......but ok, peace.

And I think I know the answer to my question as to why the pattern can't be edited to pattern in the second dircetion. It can. It's just I was trying to select the opposite direction on the Y axis as the "second direction", and the pattern function recognizes that as the same direction. If I select any edge of the cube not parralel to Y axis as the second direction to pattern, it does so. If I want an additional pattern from same seed geometry in opposite direction on the Y axis, I just need to use a second pattern to do so.

That all helps. Thank you.

Best,
Kelly