Sketch driven pattern 1

[CADone]

Hi,
In a part file how to have a cut feature (sq cut) custom patterned as per a points defined in a separate sketch.

Solidworks has this feature and its called a sketch driven pattern.

Pl help.

Thanks
C1

 

[rollupswx]

Attach the file here. Inventor the Rectangular feature pattern is really a misnomer - it should be called Curve Driven Pattern (where the curves often happen to be straight lines - ie rectangular).

Autodesk Inventor Certified Expert
Certified SolidWorks Professional

 

[rollupswx]

Other options are iFeatures or Punch tools (which can be used to "cheat" even when the part is not sheet metal).

 

[CADone]

I am sorry,
I am unable to attach company file. How ever, Can we not pattern using just points.
For eg. say, I have one hole and need to pattern it to various other locations spcified by points in a separate sketch.
thanks
C1

 

[rollupswx]

If you create your sketch point pattern in advance of running the Hole command Inventor will automatically select all of the sketch points to place the holes. (You can Ctrl unselect any you don't want.)

Can you post an example file that doesn't include any proprietary information but exhibits all of the behavior of your private work?

 

[CADone]

I will attach one by EOD. In my case its not a hole command. Instead its a rectangular cut extrude.

 

[rollupswx]

>Instead its a rectangular cut extrude.

Depending on your need the "cheating" method with Punch might be easiest. It is almost always better to pattern a feature rather than a sketch - in either program. But without an example file it is difficult to recommend best method.

 

[CADone]

Thanks for your valuble tips. I am sorry that I am comparing to SW, because thats what I was using in my previous comp.
I have uploaded the part with my question. I have 2 questions.

1. The rectangular slot Extrude2 need to be patterned at all the point locations in sketch3.

2. I use this part in an assembly with another similar part having round holes in the same location and I need to bring in fasteners in the hole location. In solidworks i have seen that there is feature driven pattern, It makes life so easy to use the hole pattern in the part to pattern the fasterns in assembly. Is there a way to do this in inventor.

Thanks
C1

 

[mcgyvr]

#1-Use Punch tools. It is easy to create a single rectangular tool that you can easily modify the rectangle size upon placement into your sheet metal part.

#2-assuming you don't have 64 bit inventor 2009 download kwiksert

http://www.kwikmcad.com/icode/addins.asp

also see here

http://discussion.autodesk.com/forums/thread.jspa?threadID=700979&tstart=30

 

[CADone]

Thanks for your response. I have a 32bit 2009. How can I upgrade to 64bit? Should I need to buy or upgrade.

 

[mcgyvr]

umm I guess I confused you.
Addins like kwiksert have not been updated for use on 64 bit systems.. So thats why I said as long as you don't have 64 bit inventor then download kwiksert.. (Kwiksert is for 32 bit operating systems only at this time)

To answer your 64 bit question. You need to change your operating system (and probably whole computer to one that is compatible) to Microsoft Vista 64 bit or XP 64 bit then when you install Inventor it will automatically detect the 64 bit operating system.
So on your Inventor 2009 DVD it has both the 32 and 64 bit versions (so you already have it but don't have the operating system/hardware to support it)

 

[rollupswx]

It looks like the Punch solution will work for you. It does not matter if the part is actually sheet metal or not.
The key to creating a Punch tool is that 1) it must be intially created on a part face rather than a workplane and
2) it must have a sketch point in the first sketch to indicate where to place on subsiquent sketches. Thus a sketch point based pattern solution.

 

[CADone]

mcgyvr,

I still have a question in your answer for #1.

You suggested to use punch tool for rect-slot. How can I get it to be patterned at those points I used in my part that I uploaded.

Do I need to create spline passing thru those points?

Kindly guide me.

Thanks
C1

 

[mcgyvr]

Well first get a working (adjustable size)rectangular punch tool. (look in the help for how to create one)

Then the way you do it is create 1 sketch with simple center points (just like if they were going to be holes or whatever) then finish the sketch and pick the rectangular punch tool you just created. It will automatically select all the center points you just created in the first sketch.
Rotate and adjust the rectangular punch tool if necessary and click ok. Done all points you created become rectangles

 

[CADone]

Thx a lot.

 

[mcgyvr]

http://files.engineering.com/getfil...752-4b5f-968c-54d5913ecf06&file=Rectangle.ide

Here is the sheetmetal punch. Just place it in the location shown in "tools..application options..iFeature tab..Sheet metal punches root" location

 

[brengine]

I miss the Sketch Driven Pattern since moving to Inventor as well (compared to SolidWorks and Catia). I will try these other methods (mentioned above) out as soon as I can as well.

Thanks,
Ken

 

[CADone]

Hi all,
Thanks for your support for the users migrated from SW. Here is a situation.

I have created an assly with a sheet metal part with puched holes. I need to use a pattern feture and bring bolts in these holes. component patter feature doent allow me to select the puched holes for reference.

Will this method work. I need bolts in all the puched holes? See uploaded file (delete) for more details.

Thx
C1

 

[mcgyvr]

hate to say it but I believe your going to have to do each one manually.

I'd just use the mate constraint and an angle constraint.
Mate center point of proper bolt head face to workpoint you created then angle constraint to keep the head parallel.

Man solidworks must be nice...

 

[CADone]

SW is nice. At the same time there are feature (Like pattern using spline curve) that inventor has got and SW is missing them.