feature array problem

[elise_moss]

This is a toughie...I have a hexagonal plate (1.2 in sides) and I want to place a rectangular array of cylinders (.03 in dia, .0745 spacing in the x-direction, .0645 spacing in the Y-direction). I want to cover the plate as much as possible.

If I create the feature at the far left origin, out in space and perform the array. Obviously some features will be in space. (I tried the adjust to model option and that didn't suppress those occurrences).

If I create an array in the center of the hexagon, I am stuck with several blank spaces which are difficult to array.

If I was doing this in AutoCAD, it wouldn't be a problem. I could create the array easily and then just erase the unwanted objects. Of course, I could do this in Inventor Sketch mode as well, but my understanding is that this will really eat up memory.

SolidWorks (sorry, got to invoke a competitor) has a pattern tool that allows you to select points and place the feature pattern to the points...this would come in handy in this specific case.

Other suggestions or ideas are solicited.

Elise Moss
www.mossdesigns.com

[Anonymous]

I've solved a similar problem by just making a rectangular pattern that is bigger than the hexagon, and using suppress (select the pattern instance in the browser, right click, and choose "suppress") to hide them. It's not ideal, but it does work. "Adjust to model" is really there to allow the patterned instances to change shape with changes in the geometry the features are being patterned on. If your pattern is a simple case, where the face along which you're patterning doesn't change (i.e. it's a plane), and the pattern instances do not interact, I would recommend using the new "optimized" option in R9 - it can significantly improve the compute time for feature patterns. Another approach is to divide the hexagon into 6 triangular areas, fill one with your cylinders, and use circular pattern to pattern the remaining 5 triangular areas. Hope this helps Jeff (Inventor Part Modeling) "elise_moss" wrote in message news:33065384.1089936744869.JavaMail.jive@jiveforum1.autodesk.com... > This is a toughie...I have a hexagonal plate (1.2 in sides) and I want to place a rectangular array of cylinders (.03 in dia, .0745 spacing in the x-direction, .0645 spacing in the Y-direction). I want to cover the plate as much as possible. > > If I create the feature at the far left origin, out in space and perform the array. Obviously some features will be in space. (I tried the adjust to model option and that didn't suppress those occurrences). > > If I create an array in the center of the hexagon, I am stuck with several blank spaces which are difficult to array. > > If I was doing this in AutoCAD, it wouldn't be a problem. I could create the array easily and then just erase the unwanted objects. Of course, I could do this in Inventor Sketch mode as well, but my understanding is that this will really eat up memory. > > SolidWorks (sorry, got to invoke a competitor) has a pattern tool that allows you to select points and place the feature pattern to the points...this would come in handy in this specific case. > > Other suggestions or ideas are solicited. > > Elise Moss > www.mossdesigns.com

[Anonymous]

Two suggestions, First, try the new "Optimized" pattern option (available in the ">>" expanded pattern dialog). Position your original cylinder on the plate, occurrences which don't land on the plate will fail. This gives the result you want, and as a bonus it's a lot faster. The down side is that you'll get a warning dialog each time the pattern recomputes, and it will be marked Sick in the browser because of the failed occurrences. Also, if you center the cylinder in the plate, I think you'll need four patterns to cover the whole plate. The other possibility is to "create the feature at the far left origin, out in space", then after the pattern, use an Extrude Cut to remove the excess occurrences. This may not be possible if the part contains other geometry that would be affected by the cut. It will also leave partial cylinders where occurrences fall on the boundary of the plate. You can suppress pattern occurrences as Jeff suggests, though that will be a bit tedious with such a large pattern. Tom Sturtevant Inventor Part Modeling "elise_moss" wrote in message news:33065384.1089936744869.JavaMail.jive@jiveforum1.autodesk.com... > This is a toughie...I have a hexagonal plate (1.2 in sides) and I want to place a rectangular array of cylinders (.03 in dia, .0745 spacing in the x-direction, .0645 spacing in the Y-direction). I want to cover the plate as much as possible. > > If I create the feature at the far left origin, out in space and perform the array. Obviously some features will be in space. (I tried the adjust to model option and that didn't suppress those occurrences). > > If I create an array in the center of the hexagon, I am stuck with several blank spaces which are difficult to array. > > If I was doing this in AutoCAD, it wouldn't be a problem. I could create the array easily and then just erase the unwanted objects. Of course, I could do this in Inventor Sketch mode as well, but my understanding is that this will really eat up memory. > > SolidWorks (sorry, got to invoke a competitor) has a pattern tool that allows you to select points and place the feature pattern to the points...this would come in handy in this specific case. > > Other suggestions or ideas are solicited. > > Elise Moss > www.mossdesigns.com

[Anonymous]

This problem points out some improvements that could be made to the pattern tools (both feature and sketch).
I patterned a sketch point and then rotated the hex to make it easy to select the points to suppress, unfortunately you can't see the results until leaving sketch mode (at least in v8) so it makes it difficult to tell what elements you have suppressed and as you pointed out you can't simply delete a point like you would in ACAD.
Alternatively you could hold down the Ctrl key and unselect points for the holes.
I assume the actual part will be made by pressing pegs into holes - I can't imagine machining pegs as part of a plate.
If you really need to have cylinders as part of the hex plate you might be able to change to the sheetmetal environment and insert as iFeatures on the points using the punch tool (just make sure your point sketch plane is a selected face of the part and not one of the basic workplanes.

[elise_moss]

I appreciate some of the suggestions. I tried creating a triangle and doing a circular pattern about the Z-axis (having the hexagon centered on the origin), but I could not get the pattern to appear properly...using a count of 4 and a 360 degree angle, I only got a pattern on the right and left sides, not the top and bottom. Not sure why that happened.

When creating the feature in the far left origin and patterning as a rectangle, I could suppress all the features except for the original (which was, of course, out in space). If I perform a cut through that feature, the entire pattern messes up.

Your solution...to perform the array in sketch mode rather than feature mode is probably what I will end up with...thanks for the sample model!

[elise_moss]

I tried your suggestion of making a feature pattern and rotating it...as you can see from the image...it doesn't work properly.

In this example, I created a sketch with a pattern of circles, the pattern was slightly undersized and then manually created circles to fill in the spaces. I created an extrude by painstakingly selecting each of the desired circles and ignoring the ones I didn't want. I then rotated about a placed axis.

I'll try again with a triangular pattern and see if it yields better results, but I think not.

[Anonymous]

I'd have to see a picture of your circular pattern (or the part) to see why it might have failed. It should work, as far as I know. As far as the rectangular pattern, and the inability to suppress the original, I ran into the same problem. I got around that by using the geometry of the hexagon for the pattern direction, (the directions do not have to be perpendicular) so the original feature does not need to be suppressed (and also fewer instances need to be suppressed). See the attached picture. But, sketch pattern also will work, and is a perfectly valid option, if the pattern is not too huge. Jeff (Inventor Part Modeling) "elise_moss" wrote in message news:24335047.1090010230726.JavaMail.jive@jiveforum1.autodesk.com... > I appreciate some of the suggestions. I tried creating a triangle and doing a circular pattern about the Z-axis (having the hexagon centered on the origin), but I could not get the pattern to appear properly...using a count of 4 and a 360 degree angle, I only got a pattern on the right and left sides, not the top and bottom. Not sure why that happened. > > When creating the feature in the far left origin and patterning as a rectangle, I could suppress all the features except for the original (which was, of course, out in space). If I perform a cut through that feature, the entire pattern messes up. > > Your solution...to perform the array in sketch mode rather than feature mode is probably what I will end up with...thanks for the sample model!

[Anonymous]

Elise, Like Jeff suggested, you can erase the cylinders that don't land on the plate. The way I would do this is just create a sketch on the bottom face of the plate. Then create an Intersection Extrusion to the top of the cylinder. This will effectively "erase" the extraneous cylinders: You may need to change where the origin of the pattern starts to keep the cylinders from getting shaved in the Intersect. Hope this helped! :) Hugh Henderson (Inventor Workflow QA) "elise_moss" wrote in message news:12594535.1090012396817.JavaMail.javamailuser@localhost... > I tried your suggestion of making a feature pattern and rotating it...as you can see from the image...it doesn't work properly. > > In this example, I created a sketch with a pattern of circles, the pattern was slightly undersized and then manually created circles to fill in the spaces. I created an extrude by painstakingly selecting each of the desired circles and ignoring the ones I didn't want. I then rotated about a placed axis. > > I'll try again with a triangular pattern and see if it yields better results, but I think not. Attachment not added (too many attachments): "complete.jpg"

[Anonymous]

I tried adding pins with the sheetmetal punch tool and it worked fine for a handful of points. Then I tried it on the pattern of points and the computer choked. I don't understand why adding placed hole features negative cylinders) works, but adding cylinders doesn't.
I tried variations of some of the other suggestions but got bogus models (keep in mind I am using v8 and my machine is underpowered and un-certified graphics card).

[elise_moss]

Right, my system is currently choking as it tries to calculate this array. My CPU is a 2.8 GHz and I have over a meg of memory. Inventor has been thinking on this problem now for over thirty minutes.

Obviously, holes are easier than cylinders, but still....

[elise_moss]

I give up...I just could not get it to work....Inventor continued to choke, even though I have a pretty well-powered system. I think I will try using a texture...it will create other problems for me...I won't be able to fully test my model, but at least I won't have to sit for over an hour and watch the hamster run in the wheel.

Disappointing to say the least.

[Anonymous]

We made a huge performance enhancement in R9 for large feature pattens. The thirty minute wait should reduce to about thirty seconds. Sorry, I don't mean to tease. :) The way I would approach this if I was still working with R8 would be to: 1) Create a new assembly 2) Place the hexagonal plate as a component in the assembly 3) Create a cylinder component and place it where you would like the pattern origin to be 4) Create an Assembly Component Pattern of the cylinder part 5) Start a new part and derive the assembly Best regards, -Hugh "elise_moss" wrote in message news:13754041.1090015954893.JavaMail.javamailuser@localhost... > Right, my system is currently choking as it tries to calculate this array. My CPU is a 2.8 GHz and I have over a meg of memory. Inventor has been thinking on this problem now for over thirty minutes. > > Obviously, holes are easier than cylinders, but still....

[Anonymous]

6) Then do the Intersection Extrusion of the hexagonal profile "Hugh Henderson (Autodesk)" wrote in message news:40f85e21$1_2@newsprd01... > We made a huge performance enhancement in R9 for large feature pattens. The > thirty minute wait should reduce to about thirty seconds. > > Sorry, I don't mean to tease. :) > > The way I would approach this if I was still working with R8 would be to: > > 1) Create a new assembly > 2) Place the hexagonal plate as a component in the assembly > 3) Create a cylinder component and place it where you would like the > pattern origin to be > 4) Create an Assembly Component Pattern of the cylinder part > 5) Start a new part and derive the assembly > > Best regards, > > -Hugh > > "elise_moss" wrote in message > news:13754041.1090015954893.JavaMail.javamailuser@localhost... > > Right, my system is currently choking as it tries to calculate this array. > My CPU is a 2.8 GHz and I have over a meg of memory. Inventor has been > thinking on this problem now for over thirty minutes. > > > > Obviously, holes are easier than cylinders, but still.... > >

[Anonymous]

Were you trying to do this pattern as a sketch pattern? If so, it is a known issue that sketch pattern, for large number of instances, can be very slow. In those cases, feature pattern (especially with the new "optimized" setting) is probably more efficient. Jeff Strater (Inventor Part Modeling) "elise_moss" wrote in message news:13754041.1090015954893.JavaMail.javamailuser@localhost... > Right, my system is currently choking as it tries to calculate this array. My CPU is a 2.8 GHz and I have over a meg of memory. Inventor has been thinking on this problem now for over thirty minutes. > > Obviously, holes are easier than cylinders, but still....

[bill.costello]

Jeff
This has got ne curious, I tried this array and used the edges of the hex plate (mine is in mm) and I get the message, that it may take a while, it tooh less than 10 secs to create an array far larger than I needed, then I extrude with Cut the instances I did not need, again a few secs. I am only using a Sony Vaio 2.4Ghz laptop and 512Mb ram. I don't consider this to be slow. In IV8 when I have tried arrays of this nature they take for ever. I am happy with the speed of IV 9. Maybe you can answer why my pattern does not follow thw edges of the hex for direction 2?

regards

Bill

[bill.costello]

Ignore that stupid remark, of course they won't follow the 60 degree pattern when I have different direction and direction 2 values.
Anyway the array still works fine and that would be my workaround, fast and simple!

regards

Bill

[elise_moss]

I tried it both ways as a feature and as a sketch pattern. Both ways caused Inventor to crash. I ended up going back to AutoCAD, creating the part as a 3D solid and then importing it back into Inventor as an sat file/dumb body. Then Inventor was happy.

I spent at least six hours trying different methods to get Inventor to create this feature and it just simply didn't work. 😞