Multiple cut features from one sketch

[cqualley]

Quick design question. I watched quite a few tutorial videos and have completed a fair number of projects in fusion 360 so far with success. So, I'm familiar with designing using components, and I've done a reasonable amount in the CAM side of things. For some reason, I'm stuck on the best approach to replicate cut features in a body. I have a dash panel that will require multiple gauges of the same size, with the same hole layout. If I place all of the elements in a single drawing, it gets very tedious to try to move around each individual gauge hole when I make adjustments. It's difficult to try to grab all of the drawing elements without accidentally moving the incorrect drawing element, if that makes sense.

My question is, should all the gauge holes be on separate drawings, separate components, or is there some other way such as referencing a single drawing for multiple cut features. I know how to replicate components or bodies from a single drawing, but I don't think that's works the same way for cuts. I've attached a couple of screen shots of my current project, as well as one of my past similar projects.

[mango.freund]

hi, @cqualley I would never derive cam from sketches because there will always be conflicts if a sketch (hole) has not been executed (extruded). please inform yourself in these videos. components give all dimensions x / y / z exactly and the selection options (more visible) are quick and reliable. 

https://www.youtube.com/c/AutodeskFusion360/search?query=cam

greetings mango

[etfrench]

I tend to use one sketch for something like this.  Use patterns whenever possible. In the bottom image, I would model the upper left large opening and the four mounting screw holes. Dimension and constrain these before moving on.  Use a 3x2 rectangular pattern with the lower left item suppressed.  Sketch the other openings and mounting screw holes plus the extra cutouts in the two right hand openings.   Edit the dimensions to move openings around.  You can do this in the activated sketch, the closed sketch with "Show Dimensions" toggled, or in the User Parameters dialog.  When a sketch is fully constrained, it is hard to accidentally move something.

p.s. Drawing in Fusion 360 is not the same as a sketch.  It is a technical drawing.

[cqualley]

I tried using a pattern, but wasn't able to exclude the bottom left hole. The suppress option would definitely help. I think turning off dimensions would be helpful too since they just get a little in the way sometimes. 

That strategy isn't too far off what I'm already doing, so thanks for the help. 

[cqualley]

I'm sorry but I don't understand what you mean by you wouldn't derive cam from a sketch. I'm always extruding and using the hole tool prior to cam for this project. The only cam that directly references a drawing is when I engrave with the trace function. 

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[cqualley]

I think my question probably really comes down to how do I constrain the points on the sketch to lock to the circle. I'm using sketch points, then coming back and using the hole tool since that allows me to do counterboring. I haven't figured out and efficient way to constrain the points so that they move with the Interior Circle. I feel like with enough dimensions and constraints I can eventually get there, but this seems like with a center rectangle or Center Circle it should be super easy, but I can never get the points to constrain to the circle. If I could lock the points to the circle, then I could just move the circle with dimensional constraints without any issue.

I've attached a file on what I'm referring to.

[TheCADWhisperer]

If  you drag the circles (in your sketch) - what do you observe?

If you drag any of the three corner points EXCEPT the point in lower right corner (in your sketch) - what do you observe?

You need a coincident constraint between the center of the rectangle and the center of the circles.

You need at least 1 (maybe 2) coincident constraints between two of the corners of the rectangle and the desired circle.

You do not really need to create those sketch points (simply use the corners of the rectangle).

I suspect you are missing several other critical concepts - you should Attach the file from 3rd image of your original post.

Drag the centerpoint from Sketch2 in the Attached file.

What do you observe?

[cqualley]

Thanks for the information, your example works fine. I guess you're right, I really don't need sketch points at all, I can just model the holes right on the corners of the square. Previously I was only using two circles, the square makes it a little easier.  If I just use the Square and outer circle construction lines, you are correct I can move everything around together. That definitely makes it a lot easier.

I think the biggest learning curve in fusion is that you can do everything 15 different ways. There are just a lot of times when I feel like there is definitely a better way, and I'd rather learn the right way rather than some way that takes five times as long.

Just to clarify, the two different screenshots of my original post are two different projects. The third picture is one I previously did, I'm doing a second one and I wanted to do it a little bit more efficiently this time around. I'll go ahead and attach the file for the first one I did, feel free to comment on anything you think could've been done better. There aren't a lot of dimensional constraints because most of the adjustments were just made after test fitting (e.g. hole 1, 5mm to the right). The rounded nature of the part also makes it a little difficult for some of the dimensions. Also, I was working off a canvas rather than existing dimensions.

[etfrench · Accepted solution]

The screencast shows how I would sketch the larger openings.  When creating the extra cutouts on the two right hand openings, don't trim the circles.  Just select both boundaries when extruding.  I've found that control point splines are easier to manipulate than fit point splines when matching an image.

[cqualley]

I appreciate it, that's very helpful. Thanks for taking the time!