How to modify a sketched rectangular pattern [Inventor 11]?

[Steve Bahr]

I created a solid of length 'x', sketched a rectangular pattern [slots] on one face of the solid, then extruded the sketch. Later, I discovered I needed to make the solid longer, but I cannot modify the sketch to add more slots; nor can I modify the feature. I tried deleting the sketch to make a new rectangular pattern from a feature, with no success. Thoughts, anyone?

[Anonymous]

Try right-clicking on one of the pattern instances, you should see and "Edit
Pattern" option.


--
Andrew Faix
Product Designer
Autodesk Inventor
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DIGITAL PROTOTYPING - Got it?

wrote in message news:5662345@discussion.autodesk.com...
I created a solid of length 'x', sketched a rectangular pattern [slots] on
one face of the solid, then extruded the sketch. Later, I discovered I
needed to make the solid longer, but I cannot modify the sketch to add more
slots; nor can I modify the feature. I tried deleting the sketch to make a
new rectangular pattern from a feature, with no success. Thoughts, anyone?

[Steve Bahr]

Thanks, Andrew. Your suggestion worked.

[JDMather]

>I tried deleting the sketch to make a new rectangular pattern from a feature, with no success. Thoughts, anyone?

That sounds like a different problem. In general it is usually better to patter a feature than pattern a sketch.
Can you post the file?

[Steve Bahr]

Thanks for your reply, JD. However, Andrew's suggestion did work for me, and all I needed to do next was edit the feature to include the new slots. I will keep your suggestion about patterning a feature, rather than the sketch, in mind when I need to do this in the future.

[Anonymous]

J.D.:

For what reason do you suggest patterning features rather than sketches?
I'm not suggesting that your wrong, just wondering what your reasoning is
for your suggestion.

wrote in message news:5662391@discussion.autodesk.com...
>I tried deleting the sketch to make a new rectangular pattern from a
feature, with no success. Thoughts, anyone?

That sounds like a different problem. In general it is usually better to
patter a feature than pattern a sketch.
Can you post the file?

[JDMather]

Here are just a couple of examples

Create a circular pattern of sketch centerpoints for a bolt hole circle and then exit sketch and place the holes. Now go back and edit the sketch to increase or decrease the number of sketch points. Rebuild. The number of holes does not change.

Create a pie piece shaped sketch. Extrude and then circular pattern the feature.
Do the same thing except change your radial lines for the pie piece to construction lines and pattern the arcs in the sketch.
If your lucky you won't get a redundant coincident points error when you try to extrude the sketch. Now try this with experiment with something significant - like a gear or sprocket tooth profile. Have fun.

There are times when a sketch pattern make sense but whenever a feature pattern will create the same geometry opt for the feature pattern. The simple sketch will be much more robust than the complex sketch pattern and the pattern will be much easier to edit.

When you create a sketch pattern think of all of the constraints that Inventor must keep track of. For example imagine the profile of the gear tooth or sprocket tooth suggested earlier. Normally I test a sketch by trying to drag endpoints. All of the relationships of those sketch entities in a patterned sketch must be calculated by the computer.

I have seen many many other examples. Maybe someone else has some good ones.

Again, I did NOT say never use sketch patterns. If I don't emphasis that I'm sure someone will want to interpret that I did.

[swalton]

If you create bolt holes with a sketch pattern, the pattern component tool in the assembly mode will not recognize the pattern and populate all the holes.

If you create the same holes with a feature pattern, the pattern component tool will recognize the pattern and populate all the holes.

This is a significant time saver when placing several hundred rivets in matching holes.

[neil.hamilton]

This is really helpful.