How to place a hole offset from a line?

[jimerman]

I am trying to create a hole pattern in a simple rectangular board material.  I created my board body, and placed a hole.  But now I want to locate that hole at a precise offset from each edge.  But I can't figure out how to do that.  If I select the hole and a line on the edge of the part, it doesn't let me modify or insert a constraint.  Right-clicking on the hole or line doesn't seem to give me anything useful here.  What am I missing?  For example, I want a hole in the corner, 1 inch from each edge.

[taylor.stein]

Hey Jimerman,

I typically approach this problem as a two-step process:

1. First, I create a sketch on the rectangular surface. In this sketch, I dimension a single circle - its diameter and any necessary dimensions from edges. 
2. Stop the sketch and extrude this circular profile the desired amount to create the hole. If you only want one hole, you're done! If you want to pattern this hole around your part there's one more step. To do this, I'll use the Rectangular Pattern command (Create -> Pattern -> Rectangular pattern) to pattern the extrude feature around my part. In the Rectangular pattern dialogue window, I'll typically change the Pattern Type to Pattern Features and select the feature I'd like to pattern from the timeline at the bottom (the extrusion in this case). 

Let me know if you have any other questions!

Taylor

[NicolasXu]

Hi jimerman,

Besides the workflow Taylor mentioned, there is another approach to control the offset of hole center from edges. When creating or editing hole, select the center mark manipulator of the hole to activate it, then you can select points, lines, and edges for location references.

You may also search "Hole" from the Help drop-down, which will list more related topics in a web browser.

Best Regards,

[jimerman]

Thanks Taylor and Nicolas. I must admit, my end goal was to create a hole, then pattern it, and I left that detail out. For example, in CATIA I create my extrusion first, then knock a hole in the body, then take my hole and create a pattern. Nicolas, how do you select the hole center? It is a point in CATIA, but in Inventor Fusion I do see a small handle on one edge of the top circle of the hole. Selecting that doesn't seem to get me the center. Thanks for your replies.

[NicolasXu]

Hi jimerman,

It looks like you are running Inventor Fusion. I thought you were talking about Fusion 360. Sorry.

Unfortunately Inventor Fusion is no longer supported. Fusion 360 is the latest product iterated from Inventor Fusion. You will find lots of improvements in Fusion 360. If you are interested you can find out more and download a free trial here: http://fusion360.autodesk.com 

As for your question, the Hole Center Manipulator is the small sphere at the center. Click it then select edge to add reference.

Regards,

[karyeka]

Here is the video I had done for some other thread - https://screencast.autodesk.com/Main/Details/a92ba64d-203b-4dfd-96fe-420275c2fb04

I hope this helps, please let us know if you have any questions.

Thanks,

Anand

Fusion360 Development

[NicoleAglaris]

Nicolas,

      I´m using Fusion 360 but I can´t seem to find or access the Hole Center Manipulator either. Could you provide more details on exactly how to get there from a hole or extruded circle? Clicking on the center mark doesn´t seem to do anything, and if the hole was created with the hole command sometimes there is no center mark to click on. 

Taylor,

       When I tried your method I ran into the same problems as jimerman, my intuition is to select the center of the circle and the edge, but this doesn´t allow me to modify the dimension or enter in a constraint. How do I enter the desired distance from an edge?

Thanks,

Nicole

[NicolasXu]

Hi Nicole,

The video in Anand's reply shows the details of the steps. When creating or editing hole, we can click on the center then click on edges to add the reference. 

Please let us know if there is any questions. 

[Lonnie.Cady]

The problem that all holes are not dimensioned from the edges of squares.

Show a video with a hole dimensioned from another hole or a circular boss or a radial hole pattern.

I have tried adding sketches and snapping to sketches points but the hole does not stay attached to the sketch point if it is moved.

We need to see some videos and techniques that are not a hole on a square box dimensioned from the edge.

[karyeka]

Here is a video where I am using sketch points (which are dimensioned of other points) to center my holes. Later I update dimensions to change those sketch points and correspondingly holes. https://screencast.autodesk.com/main/details/a7839aed-5aa9-4a52-be8f-0fe8458645d3

If I just drag those sketch points or even move them using the Move command the holes don't update. Huum, this should work and we will look into this. It seems only dimension update is honored by the holes at the moment.

Not an elegant but nevertheless still a workaround - I created sketch circles instead of just sketch points and those work nicely. The holes update when I edit dimensions, drag them or move them using Move command.

https://screencast.autodesk.com/main/details/0213d4df-9a4f-4bd3-ad69-622cdc44667a

please let me know if you have any questions.

Thanks,

Anand

Fusion360 Development

[Lonnie.Cady]

I tried it again with no luck.  I just used a square and realize I could have just added reference to the edges from the hole command but just wanted to try the method your video showed with a dimensioned sketch point and I did not get it to work.  I must be missing a step somewhere.

https://screencast.autodesk.com/Main/Details/51c10494-098f-47e7-8aec-b80feb198be8

[schneik-adsk]

When you edit the hole, clear the face selection in the dialog by clicking the red, "X."
Then select the sketch point.

I think that is the missing step.