Editing geometry of a pattern

[cvriv.charles]

Say I have a circular pattern that consist's of 6 circles. Say I want to cut one of those circles in half. How do I do that? If I try to trim it wont let me. Do I have to create 6 circles in a circular pattern manually? This is just a simple example of what im really trying. But the concept is the same.

 

Thanks in advance.

[cvriv.charles]

Ok. Been messin around with this and i found a way, kinda. But still leaves me with questions. I attached a simple example.

 

In sketch1 I had drawn a circle and within this circle are 6 smaller circles in a circular pattern.

 

I then created sketch2 and projected the geometry of sketch1. So in sketch2 I have whats in sketch1 except with the green projected lines. I then chose a circle drew a line through it and then created an arc for the half I want to keep. I then delete the green projected geometry for that circle only. Then I extrude the whole shape.

 

There has to be an easier way. The actually model in working on is alot more complicated than this example.

 

QUESTION#1: First, can I avoid all this by editing something in a pattern directly?

 

QUESTION#2: Is there a way to mass select geometry to be projected as oppose to projecting each line individually?

 

QUESTION#3: When I do have the geometry projected, I cant work with those green lines as if they were normal lines. Example, I cant split, trim, etc. If I have to alter a section of geometry, I have to redraw that geometry using the green projected lines and then when done I delete the green projected lines. Anyway to upgrade those green projected lines to normal lines without having redraw?

[shift1313]

okay im a little fuzzy on what you are trying to do. Do you want to only "half" certain circles, only 1 of them or all of them? The better method is to create one circle, then pattern that outside of the sketch.

 

Q1. in this case if you drew a vertical line through the red(projected) circle you would not need to trim anything. Inventor is really good about letting you select what you want to extrude.

 

Q2. If you use the Project Geometry button then select a face rather than an edge, it will project everything on that face.

 

Q3. You can break the link of projected geometry but then you loose the benefit of projecting it. To break the link, right click on the line you are dealing with and about 3/4 of the way down the pop up list you will see Break Link.

[cvriv.charles]

Well,.... what im trying to do is edit the pattern as a hole. The example of circles is very simple. In the example I was only trying to edit one circle to try and figure this out. I'll attach the actual file that im working on. I found a way around this. So you can see what I am really trying to do.

 

Im sorry. And also,... what if your trying to project geometry from one sketch to another. I know that if I create all the circles and then extrude and then create a sketch off the face all the geometry for that face will be projected. I can then edit the projected geometry and then extrude again filling in the original extrusion with the changes. Just like what I did in the second attachment. I know there is no right or wrong way of doing it but seriously,... theres got to be a way to do it easier than that. I would like to be able to do it all in one sketch. Create the pattern and then cut away from the pattern with some other geometry or something.

[JD Mather]

I know there is no right or wrong way of doing it but seriously,...

 

I would NEVER do a pattern like you have done in Sketch3.

 

It is almost always better to pattern a feature rather than a sketch.

 

Do this experiment -

Edit Sketch3

Right click in the graphics window and select Show All Constraints.

[shift1313]

At a first glance this is probably how I would approach the model. Draw the plate as you did. Then extrude cut the negative space(speaking of the outer ring), but only cut the top half. Add a "spoke" and then array that feature. then mirror the top half down.

[cvriv.charles]

Thanks for the tips. I will try them as soon as I can get back to my computer. Thanks again.

[cvriv.charles]

Awesome! Check it out. Tell me what you think. I used your technique shift but a bit tweaked though. I really needed the .0625" radii for the "spokes". So I had to improvise. Let me know what you think.

 

Now im off to the next step. This is only the begining for this design, lol. So complicated. It was so much easier in SketchUp. But I am loving the dimensioning/ constraining of inventor though. Its challenging:) Like a puzzle.

[cvriv.charles]

Ick. Cant say I like how its turning out. Going to have to make some changes. But this was the next step. I had to draw half of it manually. Then mirror the other half. Was wondering if there was a better way? Again,... the corner radii are needed. This is a great learning experience. Im really enjoying this. Oh I couldnt attach the file because now its greater than 250k. Heres a pic though.

[cvriv.charles]

Forgot. I'll email the file if you guys want to play with it.

[JD Mather]

Oh I couldnt attach the file because now its greater than 250k. Heres a pic though.

 

Did you drag the red End of Part marker to the top of the browser before saving and zipping?

 

Also, You might experiment with the Grill feature on the Plastics tab.

[shift1313]

In your sketch 3 I wouldnt draw any of the spokes. In your array your spokes actually go over the ones already there. I would also avoid fillets in the sketch but rather do them as features and then include them in the array.

 

From the looks of the part it appears you are making a dual fan grate? I cant recall if this was added in 2009 or 2010 but there is a Grate function and also a Rule Fillet option that would help with this kind of thing. You could knock out all of the fillets in one shot.

 

It might seem counter-intuitive but i would probably start by subtracting your 3rd "opening" first.

 

dont pay too much attention to the features i made because I did this in a hurry but thats the general idea.

[cvriv.charles]

Did you drag the red End of Part marker to the top of the browser before saving and zipping?

 

Also, You might experiment with the Grill feature on the Plastics tab.

 

I did move the EOP up under origin before saving. I remember from the last time you told me to do so;)

 

The grill feature on the plastics tab? Will have to search for that. Thanks.

[cvriv.charles]

In your sketch 3 I wouldnt draw any of the spokes. In your array your spokes actually go over the ones already there. I would also avoid fillets in the sketch but rather do them as features and then include them in the array.

 

From the looks of the part it appears you are making a dual fan grate? I cant recall if this was added in 2009 or 2010 but there is a Grate function and also a Rule Fillet option that would help with this kind of thing. You could knock out all of the fillets in one shot.

 

It might seem counter-intuitive but i would probably start by subtracting your 3rd "opening" first.

 

dont pay too much attention to the features i made because I did this in a hurry but thats the general idea.

 

I will have to look for those features and try them out. This type of modeling with INV is proving tideous:( And you are right. I am making a 2x120 radiator grill:)

[cvriv.charles]

Ok I dont think 2009 has any grate, grill, or plastic features. I did a search in the help and nothing ame up. I googled and saw 2010 everywhere. So sucks to be me.

 

On the other hand,... totally forgot about the fillet feature for solids. OMG,... I filleted everything in a nanosecond. LOL. And there I was farting around drawing them all.

 

In sketch3 I drew the spokes so they would have the correct fillet. Dont have to worry about that now.

[shift1313]

When you are modeling something like this always think about the different ways you can approach the shape. For instance in your original couple images you were subtracting the holes which (as you found) is a lot of work and editing that is nearly impossible. Cutting the entire hole out and adding back the ribs making use of rectangular and circular patterns is a much easier, faster and more robust method. Also keep in mind if you dont want to use circles, rectangular pattern can follow spline curves.

[cvriv.charles]

Also keep in mind if you dont want to use circles, rectangular pattern can follow spline curves.

 

Really? I actually tried to find a feature like that. A real quick try using the rec pat tool and I thought it wasnt possible. I will have to try that again.

[JD Mather]

Ok I dont think 2009 has any grate, grill, or plastic features. I did a search in the help and nothing ame up. I googled and saw 2010 everywhere.

 

Oops, forgot that you are on 2009, yes Grill and Rules Fillet was added in 2010.

 

I guess you saw from the little experiment that i suggested why to only use patterned sketches when absolutely necessary - all of those constraints Inventor has to solve and can drag a system to its knees as well as being more difficult to edit.

[cvriv.charles]

I guess you saw from the little experiment that i suggested why to only use patterned sketches when absolutely necessary - all of those constraints Inventor has to solve and can drag a system to its knees as well as being more difficult to edit.

 

LOL. Yes, that I noticed. My computer is pretty beefy and yet it INV was still crashing.

[cvriv.charles]

Phew. Done. Needs tweaking though. Just doesnt feel right. Anyways,... was a great learning experience. Sequence is very important. Still cant upload the latest file. Size is 301k.

 

Anyways,... I followed your techniques shift. You know the outer ring thats kind of cut, with the spokes. The two spokes towards the pointy ends kind of protruded through that ring into the rectangular pattern spoke area just a bit. So I created another sketch and kind of turn the protrusions into closed shapes so that I cut extrude/ cut off the slack. It was the only way I could think of to remove the slack. That was easy atleast. It worked.

 

This is great. The methods I used are WAY off from how I was initially doing it. LOL. Thanks guys:)