Curve dirven pattern - skecht entities along path

[0x3FA5]

Hi,

I am trying to pattern a point (for example) along a slot. The holes should be evenly spaced along the curve.

Cannot find the feature command, please help.

Thank you!

[Sergio.D.Suárez]

Hi, is this what you are trying to do?

I hope this helps. regards

[0x3FA5]

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@Sergio.D.Suárez wrote:

Hi, is this what you are trying to do?

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Thank you for your reply.

No, this is not what I tried to achieve, although thank you for this tip.

I am trying to equally space a sketch entity (hole, rectangle, block, etc) on the sketch level, not creating a hole pattern.

P.S.

Also, the way you recommended does not work for some reason, it is skewed:

[CCarreiras]

[Sergio.D.Suárez]

Regarding why my example didn't work, here is a review. In this example the separation is made in the measurement of arc length, not in the linear distance between centers of the cylinders.

[0x3FA5]

Deleted comment.

[Sergio.D.Suárez · Accepted solution]

On the other hand, thinking a little about the problem. I think you can't make a pattern in a sketch by taking a guide curve and maintaining the same separation.
If you need the same distance between the centers of each point, the method that I show you will not work for you (in the curve it will take the distance over the curve arc, not the linear distance). However, I would not recommend doing the pattern even if you could do it as you are proposing.
There is an alternative and very effective method, something more complex.
You must use equations and conditions.
The file I share is an old file, I did it a long time ago and it can surely be improved. It is an adaptable chain model.

Go to parameters and modify Z1, Z2 and "Desfase"

The interchanges and the diameters are changed and the chain is updated with the inserted parameters. Work with ilogic. It is an effective method because you don't have to edit anything in the sketch. When it comes to patterns, there may be problems that make it necessary to edit them when making changes

I hope this helps. regards

[0x3FA5]

Thank you for such a detailed response.

I am not familiar with iLogic at the moment, nor have the time to invest into exploring overcomplicated ways to solve such a simple issue.

This is not the first time I am encountering complex solutions in Inventor for problems, which in other CAD I would do without even paying attention.

For example, in SW this issue is not an issue and solved in 3 (THREE!) clicks.

I will select your answer as a solution.

Thank you!

[Tom_Sturtevant]

Hi –

Sketch Pattern currently only supports a linear path.  I encourage you to add an “Idea” for this (or if one exists give it +1).

One brute-force way to achieve this today is to create a pattern of work points and project them into your sketch.  There are some obvious draw backs to this approach but it will give you equal spaced sketch points without requiring you to do the math.   I have attached an example part.  The basic workflow is:

1. Create Sketch #1 with one sketch point and the path you want it to follow (note: the path curves can not be Construction geometry)
2. Create a WorkPoint on the sketch point
3. Create a (Rectangular) pattern.  Select the work point and the sketch curves, choose “Curve Length” as the spacing option, select the work point for “Direction 1 > Start”
4. Create Sketch #2.  Project each work point into the sketch.

Draw backs include

You end up with two sketches plus a work point and a workpoint pattern.

You need to project each work point: click, click, click, …  Not too bad for 10 – it will really suck for 100.

To change the number of points you need to edit the pattern, then edit Sketch #2 to project any new work points.

Really only works for sketch points, not for patterning sketch curves.

Hope that helps.

T.0.M.