How to pattern or copy

[acad-caveman]

Gentlemen, I would like to ask a very newbie question.

Attached are two files, one is an AutoCAD representation of what I would like to do and the other is the IV file I'd like to do

it in.

There is one feature that I need in 12 different locations. One is in the center, 4 of them in a .465 dia polar pattern and 7 in a .930 dia pattern around the center.

For the life of me I cannot figure out how to do it in Inventor and would lke a kick in the pants regarding what am I missing or doing wrong.

In Solidworks it is quite easy due to how SW uses "hole" features by way of a double sketch ( profile sketch and location) . I was thinking IV has an equally simple but different way of doing it ..... I guess I'm just not seeing it!

As the IPT shows, I've done the revolved-cut feature and tried to "pattern" it. Can't do!

I've also attempted to copy the feature. Can't do!

Could someone plese look at them both and give me a starting point?

The ACAD file is very quick and dirty but is an exact replica of what I need.

Thank you!

[JDMather]

---

@acad-caveman wrote:

In Solidworks it is quite easy due to how SW uses "hole" features by way of a double sketch ( profile sketch and location) .  

---

Something like attached?  (Oh, and please do attach your *.sldprt solution here - I would like to see how this pattern would be easier in SWx. )

[JDMather]

...and alternate solution.  (see attached).

[acad-caveman]

JD

  Thanks for the reply.

Your example is fine and I could easily do it if it was just a simple hole.

Problem is that mine is the counterbore/chamfer/through hole combo that is to be patterned.

Attached is a SW file to show the intent.

Oddly enough, their method of a "revolved cut" sketch @ point location sketch is quite nice, except in SW2007 they have

had no way of circular-array in the sketch environment.

Inventor has no way ( that I know of ) to do the similar hole using a revolved cut @ point locations, but it does have a nice 

circular array of sketch elements ( in this case points )

Before anyone gets defensive, please note that this is in no way knocking Inventor!

It is also quite possible that my lack of training is what's the issue.

p.s: I hope I'm not violating any forum rules! I had to add the doc extension to the SW file for the upload!

If this is a no-no, please delete and advise.

[IgorMir]

Here is an example for you to look at. I think Jeffrey would have done something similar (couldn't see his version, different IV releases). in the attached part modifying the Hole 1 will alter all of the holes (and chamfers) in the part. To see the effect - edit Hole 1 and change the thread definition from M4 to, say, M5.

Regards,

Igor.

[acad-caveman]

Igor

  Thank you.

That is the end result I'm looking for.

With the risk of sounding like a little baby: BUT!

What you did was created one feature and gave variables to it's dimensions.

You then created 2 separate and independent instances of the very same feature and used the previously defined

variables for the dims.

IOW you've drawn the very same and exact feature 3 times as separate features.

That too is something I've done  and knew was possible.

I guess then there is no other way ....

But what is the "Copy Object" option for?

[IgorMir]

Well, technically I didn't draw a second feature. Nor did I the first or the third one. The software did it for me. I just made sure that all the features share the same parameters.

You see, there is always a quest to find a magic button which does it all in one hit. Yet, 99.99% of those quests are failing miserably. So, I concentrate my efforts on making a simple to follow/edit and reliable models instead. If there is a better way to get done what I do - I am all ears. If not - then my way is the best way. And so far I got little to complain about.

As for the "Copy Object" tool - I had a look at it in brief but don't use it in my workflow yet. Maybe some one with better experience with this function will shed some light on it.

Best Regards,

Igor.    

[acad-caveman]

Igor, guess I might have stepped on your toe. Not intentional!

Again, nothing wrong with what you did, nor would I be in any line to criticize it if it was otherwise.

I was just simply wondering if there was a tool that would take a single feature and copy it in pre determined places as many times as needed.

In many ways, that is exactly how one does go about it in AutoCAD. I drew the hole shape just once, created the intersection points of the locations and then copy them as many times as needed.

After thinking about it, Solidwork's Hole feature - while useable in this particular case - is not a solution either, as it woudl work only with revolved-cut features. If the same thing would have been anything other than, it would also be of no use.

With that said, I guess it might be better to modify the tite of the OP by asking if it is possible to copy a feature from a base point to a point location(s) in cases where the rectangular or polar array cannot be applied.

One would think it is a relatively common task. Hole features are almost always done using this method, but why should the option be limited to that alone?

[JDMather]

Punch tool  will do this - even if the part isn't sheetmetal. 
BTW Autodesk has no problem with posting SWx files here - I would have done the SWx solution differently - too much work in your solution.  I try to avoid work.

[acad-caveman]

With the risk of beating this dead horse too much...

Could you please look at this ( i think final ) version of my attempt.

What I did was to sketch the first revolved cut and then copied it 2 times to the inner and outer circular pattern C/L.

After that I've shared the sketch, crated individual revolved cuts and then individual circular patterns.

Please ignore the fact that the dims used were explicit rather than linked, this is only a concept for possible future useage.

The idea is that since all the repeated features are identical, I now have one place where I can change both the shape and the

circular pattern diameter.

Thank you again

[JDMather]

---

@acad-caveman wrote:

With the risk of beating this dead horse too much...

... I now have one place where I can change both the shape and the

circular pattern diameter.

---

Why give up so easily?  It looks to me like you are still doing way too much work.  Why not use the Punch tool?

[JDMather]

---

@acad-caveman wrote:

Could you please look at this ( i think final ) version of my attempt.

---

Before moving on to a discussion of Punch features, I have to wonder why you didn't simply use Equal = constraints in your sketch rather than adding all those dimensions...

or

...maybe better yet, a sketch block?

[acad-caveman]

I didn't use the equal constarints simply because I was just making stuff up as I went, testing the what-ifs, but that would definitely be the way it'll be done. One place to edit and as few items as possible.

Sketchblocks ..... Did not get there in my learning quest yet, but if they are anything like ACAD's blocks, then that might even be a better solution as this item has quite a few different versions, all with the same hole shape in various, often completely random places.

As a sidenote, I do like Inventor's ability to select only a single closed sketch geo from multiple possibilities to use for a feature.

In this case, all the geometry and center axis exist in one sketch, but are used in separate revolved cuts.

If for nothing else, just learned something .....

[JDMather]

---

@acad-caveman wrote:

.... One place to edit and as few items as possible.

---

Before I work up the Punch tool example I'm trying to figure out your design intent on the SWx example you posted.
Why did you create all those extra dimensions, points and lines rather than simply to two circular sketch patterns on the first two sketch points?  (see attached)   I can think of some possible reasons, but I need to know your logic to suggest the best Inventor solution.

[JDMather]

See attached files.
Double click on the Punch feature in the browser.
You get the 4 variables size the features of the hole.
Double click on one and you get a prompt of what to do. (you can customize the prompt).
In this case you can enter any desired values, but you could set up limited table of only those values you actual use in your designs).

Exit edit of feature.
Edit the placement sketch.
You see pattern of hole locations and pitch circle diameter.
If you change the number of sketch points then edit the Punch Feature to reselect the pattern of sketchpoints.

If you want to omit specific points in a pattern - edit the feature and Ctrl select the point you wish to omit.

Create a library of custom "Punch" features your company commonly uses.  I put "Punch" in quotations as you can use this for all manner of features besides holes - don't let Inventor terminology limit your use of this tool which allows placement of about any feature to be as easy as placing a Hole.

[JDMather · Accepted solution]

Oops, I meant to toggle back to standard part.

[acad-caveman]

JD. That is the tool!

Tough I have not figured out exactly how you did that or how the punch tool works, I will be digging through the documentation and get a good grip on it.

It appears that this is in fact the method of creating a feature ( of any shape apparently ) and repeat it in any point location.

BTW the SW example was just simply to indicate that a point-location can be used to place the feature. In this case obviously a polar array would have been the better method, but for instance this part also has 6 tapped through holes that are randomly placed on different boltcircles and are dimensioned with an angular location from the Y axis. ( I'm re-creating a model from a 1963 blueprint )

Thank You again!

[JDMather]

---

@acad-caveman wrote:

JD. That is the tool!

Though I have not figured out exactly how you did that or how the punch tool works..... 

---

Hollar back when you run into trouble - I use it in ways that weren't exactly intended, so the documentation might not give you the information you need in order to use it the way I use it.  I've been on Autodesk for years to make this tool available in the standard modeling environment rather than having to toggle back and forth from sheet metal environment.

[ROBTRONIX]

---

@acad-caveman wrote:

It appears that this is in fact the method of creating a feature ( of any shape apparently ) and repeat it in any point location.

---

You may also want to try the sculpt tool for re-using complex geometry. The workflow is slightly different from using punch features in a single part file.  

You would essentially create a new part file that represents the feature you are trying to re-use.

Place this part model into the assembly that contains the target body that will receive the feature.  

Using 3d constraints position the feature model to your target body. Once full constrained edit your target body, copy object, as surface with associativity on.  Sculpt, Cut.  The feature is cut from your target body.

Try experimenting with associativity by suppressing your constraints and manually re-positioning and rotating your feature part. The cavity on the target model automatically updates.  Just remember to turn associativity off when you are done!

These sculpted features can be patterned both circular and rectangular just like regular reatures.

This will allow you to make very complex features and position them anywhere in 3d space.

I

[IgorMir]

Hi,

No, you don't have to apologies at all! My previous response to you should not be read as some what patronizing at all.

Sorry if it appeared that way. It was not intentionally be any means.

Best Regards,

Igor.

---

@acad-caveman wrote:

Igor, guess I might have stepped on your toe. Not intentional!

Again, nothing wrong with what you did, nor would I be in any line to criticize it if it was otherwise.

I was just simply wondering if there was a tool that would take a single feature and copy it in pre determined places as many times as needed.

In many ways, that is exactly how one does go about it in AutoCAD. I drew the hole shape just once, created the intersection points of the locations and then copy them as many times as needed.