Best way to creating the same extrudes

[cadbart]

Hi,

I'm creating a simple model in which there's a couple of the same cut extrudes, as follows:

Now, I've achieved this by creating one extrude, creating rounds on it, mirrorring this extrude, and mirroring the extrude and the mirror of the first extrude which is... a little complex design intent and makes a model tree hard to read.

This is horribly unreadable if you ask me... I'd love to make a Pattern from extrude, but by using Axis Pattern I got something like this:








...which is huge different than part in the first image. 

I thought about creating all mirrors inside sketch and then extruding (cuting) all 4 shapes in one operation (Extrude) but I'd really like to make it with Pattern if possible.

What do you think? What is the best way and most healthy practice to achieve this?
Thank you in advance for all answers!

[tbraxton]

The trick here is to use a datum plane to control the clocking angle of the extrude. You can then group the datum and extrusion and use axis pattern. I have enclosed a sample model (Creo 4) that has the orientation of all extrusions pointing at the central axis using an axial pattern.

Query the sketch of the pattern leader (Extrude 2) and you will see that datum 4 is used as a sketch orientation reference which will control direction of your extrude.

Use of clocking reference to orient extrusion in pattern

[cadbart]

tbraxton, thank you for your answer and files! Your way works great with symmetric shapes but when you try to make it for my shape you'll see result shown on my post's second image and I'd like to get result shown on the first image. Besides, (I'm sorry I forgot mention it in origin post), the distance between the shapes horizontally and vertically is different... So we cannot use the axial pattern. 

The thing is I don't need to use a pattern to do it - I'd just like to make it as good as possible. I'm searching for the best way and healthy practice so that the model tree and design intent will be clear.

Do you have some idea?

[KenFarley]

When I have to make some complex features that I don't want to have mirrored in the sketch, I will build the portion of the part (a quarter of it, for you) with those features, then mirror the whole part to get all the mirrors I need. I hate the inflexibility of mirrored features, plus the complexity of the model tree as you mentioned.

For your situation, I might make a rectangular block with the initial cut through, mirror that for two, and mirror again for the final set of cut through features. Then I'd cut the outer shape of the thing based upon one or more of the through cuts. But, that's my recipe, and there are a lot of other cooks in the kitchen.

I don't see an easy way to use a pattern, unless there's some way to do a rotation of the feature as it is patterned, a sort of two-dimensional pattern...

[cadbart]

Thanks for your answer, Ken! In refer to the other paragraph in your reply - could you explain, please, what exactly did you mean? The thing is I already have mirror and mirror of mirror of this extrude (making inside Model, not Sketch) but I really don't like it due to model tree illegibility... Also pattern is not gonna work because it doesn't make its elements to be mirrored. To be honest I think the fastest, the simplest, the most clear, and the easiest to update in future way in this situation is to:

• draw this shape inside sketch with all rounds,
• mirror this shape thrice inside sketch,
• then just cut it by Extrude.

In this way it'll be one operation (Extrude) in model tree containg all shapes (main shape and three mirrored) defined in sketch. 

What do you think about this idea? 

[pausob]

Hi, I'm piping in to discuss about mirrors / patterns as I'm pondering the same issues these days.

---

@cadbart wrote:

• draw this shape inside sketch with all rounds,
• mirror this shape thrice inside sketch,
• then just cut it by Extrude.

In this way it'll be one operation (Extrude) in model tree containing all shapes (main shape and three mirrored) defined in sketch. 

Given the simplicity of the provided example, this will work, but I would definitely not recommend including the rounds in the sketch.  Instead, round the feature's extruded intent edges.

So I think that if the intent is to have the same shape, reflected to be in 4 "quadrants", then all methods already mentioned will work well.  Your original method of mirroring features twice achieves the design objectives and arguably it would be the one most easily understood by all Creo users.  In my opinion, Ken's method of mirroring a whole 1/4 part is much more stable.  But I think PTC made improvements and maybe in Creo 4.0 mirror feature actually works well?

I suggest you could just polish up your original model.  Maybe incorporate rounds with intent edges (I am assuming you did not use them).  To tidy up the model tree, group the features together and make it a single collapsed node in the model tree.  Give it a name and maybe even add a note to the group to explain what is going on. 

Anyway, as I was also looking for a more general way of making translated and reflected copies of sketches, I came across 2 methods.  Perhaps they are not as straightforward, but depending on complexity of the application, these might be simpler in the end than the methods already discussed:

- Using patterns (table, or dimension) to specify instance placement - since 2D reflection of a flat shape in XY plane can be obtained by its 3D rotation by 180° about x or y axis (so those rotation angles are the dimensions that can be varied in patterns).

- Using copy and paste special functions + utilising the "apply rotation / translation" option (again, the reflection is obtained by 3D rotation).  These generate similar "copied features" as the (feature) mirrors.  So I'm not sure how stable they are in practice, but in my initial testing with Creo 4.0, drastic changes to the sketch (i.e., deleting all its entities and redrawing a completely new section) seem fine - the model regenerates without failures.

I share the example model (Creo 4.0) for demo:

I'm still evaluating which method works best when it comes to creating drawings / showing annotations in combined states.

Also, I'm interested in other people's methods of using patterns in skeleton master models and how to propagate such design information to the target models.

[tbraxton]

This is not the only way to do it but is readily understood as there are only two sketches in the model that can be edited. I think this is what Ken was proposing and I agree that it is an expedient method to create the geometry. You mirror the part by selecting the part at the top of the model tree and then the mirror function. There are other methods but this is probably the fastest way to get the desired geometry and it is easy to understand the design intent.

I am pretty sure that it can be done with patterns but it will be much more time consuming to work it out than this.

Mirror of the part and not the features

[KenFarley]

That's exactly what I was talking about. I'm afraid I was not clear about the fact I was talking about mirroring the complete part.

My personal preference, depending on the complexity of the sketch, would be to construct the geometry in the sketch for the protrusion. I say "depending on the complexity" because when the shape being multiple-mirrored gets very complex you have to start worrying about the dreaded "section has become geometrically unstable" error. Anyway, as you note, this would be the best in terms of number of features and all that.

The thing I adopted as personal policy years ago that has save me tons of "detective work" when I need to modify an old design is naming my features meaningful things, like "PLN-SEC-AA", "HOLES-MOUNTING", etc. That and limiting the number of features to the minimum necessary, makes things much more efficient for future me or someone else digging into the models.