sketching in reference to another sketch

[jcook27FELS3]

I have a body - a boxed shaped object. I need to make another box object as a sleeve that slides over the other box.

I am trying to reference the first boxes sketch, which has some useful information - like the center point of the box, to start drawing the outer box. I want to use the Center Rectangle in the second sketch to easily make  this out sleeve box shape around the first box.

I can't reference any parts of the first sketch - point corners intersecting lines - nothing. you can see in the picture first body & sketch are showing, and I am in the new component, lets call it outer sleeve - but I can't place the CenterPoint on the intersecting lines.

How can I accomplish this?

[laughingcreek]

are you using "project" to project what you need from our first sketch into your second sketch?  projected items will show up as purple in your sketch.

[jhackney1972]

Please attach your model so the Forum users can give you a clear answer.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[jcook27FELS3]

No. Didn't use project. Not familiar with that feature.

I'll have to look it up.

[laughingcreek]

when using more than one sketch, the project tools are among the most important sketch tools available.   The first 2 - project and intersect - are probably used the most, but they all can come in handy at the right moment.  

[jcook27FELS3]

John

Is it possible I can just export and attach the sketch - this is the part I am having trouble with. I can't export the whole model since I could get into a proprietary issue.

The screen capture I've attached shows the mess I've created. Thanks to the help from you and others in the forum - I am understanding the constraint feature better. Now I need to go through the existing mess and turn blue to black.

I feel I should delete some dimensions and constraints and redo them correctly. Not sure where to start ...

If there is a way I can upload just the sketch for you - please let me know.

Thanks for all the help.

[jhackney1972 · Accepted solution]

If the sketch is at the beginning of your timeline, you can simply drag your timeline marker back to it and the delete all the timeline entries to the right of it.  I doubt this is probably  the situation so the video will show you another way.  I show only one sketch in the video, but you can copy and paste more into the same new sketch if needed.

[davebYYPCU]

No we can’t have just a sketch in an export, you could reduce the file to just one sketch.

Which part of that last picture, was referenced to the origin point?

A. Nothing.  
There is not 1 black sketch line (visible).

Take another pic of that sketch, with Constraint visibility turned off, and dimensions turned on.

Sketching technique or best workflow, is to

create detail,

constrain (something to the origin)

repeat.

As you build off black articles, it will get easier to maintain and arrive at fully constrained.

You have so many Collinear constraints, means you probably are trimming too often.

Fusion doesn’t care how many sketches you make, everything in one sketch is not efficient.

Looks like you want dogbone corners.  They should be in a second sketch.

How is the last sketch relevant to the sleeve question?

Why did you not duplicate my example, I left you one blue line.

[jcook27FELS3]

Thanks John

Here is the attachment - hope I did this export correctly.

I think just about every line in the sketch is blue -

[davebYYPCU]

@jhackney1972  Be careful, your suggestion to step left in the timeline and save send, does not eliminate opening the timeline by others.  Second version much better.

might help….

[jcook27FELS3]

Sorry dave if I missed you post - I need to go back and re-read. I'm not on F360 consistently and coming back after a week or so - I may be missing responses. I need to get better at maintaining my question list so I am making efficient use of everyone's time.

I appreciate all the assistance you guys are giving.

In current model I uploaded - yes, it is not constrained to the origin - this is just my lack of understanding here. If I move the corner of that tab down and constrain to the origin - its constrained, but a large horizontal section of the wall is then under the horizontal plane of the origin - that's what I was thinking. But I guess that maybe isn't really a concern.

How do I turn off the constraint visibility?

The dog bone corners are something I need to do in a separate sketch - agreed. This is one of the things I need to fix going forward. I think I also need to be able to project for this because I want to draw sketch #2 referencing sketch #1 (basically they are on top of each other) - more for me to learn.

[jcook27FELS3]

Thanks - I've implemented John's second suggestion - copying to separate (new) sketch and exporting.

[davebYYPCU · Accepted solution]

I saw the attachment but will be a little while before I can get to it.

You don’t want the parts below origin, that’s normal, and ok.

You just make a corner point of the bottom tab, horizontal to the Origin.

You make the corner point of the side tab, vertical to the origin.  

2 steps, very likely you have done such a wonderful job with the rest of the sketch, there will be no blue items.

Edit sketch, in the side palette / panel / options, untick show constraint.

new sketch on same plane, project items you wish to use, but depends on what you want and what you have, to find the efficiency.  (bonus - purple items are fully constrained in the destination sketch)

Might help….

[jhackney1972]

Attached you will find the sketch you sent me fully constrained.  The main issue was your relationship to the Origin.  The other issue was all the corner relief circles which need to the constrained to the lead in lines.  BE SURE to review all dimensions and alignments as I have no idea what the "correct ones are.

[jcook27FELS3]

Apologies - It looks like I may have this question topic going in two different posts. Sorry for the confusion.

Please clarify: "You don’t want the parts below origin, that’s normal, and ok." - you're saying its normal and okay to have the part below the origin - correct?

Here is a screen capture - I tried using the Horizontal / Vertical constraint to put the left side tab constrained horizontally to Origin and the bottom tab (corner point) constrained to the origin vertically.

Not sure - it doesn't look exactly like your example.

Found the View Constraint toggle - thanks.

I need to do a little reading up on projecting.

Hopefully I will have time to work with this design a lot this week.

[davebYYPCU]

(Last pic)  Ok, something is wrong. (Imported sketch - timesoaker)

Normal / previous explanations will not apply to imported sketches.

Checking the file, you have more than 1 point (3) on the Origin.

Edit sketch, window select and delete all points on the Origin.  You will lose some dimensions.

Now you can make the vertical constraint from Origin to the left hand tab.  Vertical line turns black.

Make the bottom line of the lower tab - horizontal.

Now you can make the bottom tab corner horizontal to the Origin.  The horizontal line will turn black.

I did not see any errors with this set of instructions, but not my sketch so double check.

Replace the missing dimensions back onto the origin that you did have. 

Dimension the bottom corner lines to the Origin, they will turn black.

About now you should be realizing that every dog bone circle needs extra dimensions.

This is the start of a tedious process of repairing an imported sketch.  They do not save time, because all dimensions and constraints are stripped out on import.  Means you have to create them.  Worse than that, trimming the dog bone lines and arcs loses the centre point for the circle, and each one will need to be constrained with dimensions or constraints.

Might help....

[jcook27FELS3]

I think what might be better is to delete this sketch and draw it from scratch the correct way. I can reference the original sketch for the dimensions I need to redraw it.

You summarized three steps for aligning to the origin. I think I need the specifics though - what exactly am I clicking on to accomplish? I mean what constraint icon, what point, etc.

Don't understand the part about each dog bone needing extra dimensions. When I redo it - i know I need to make those circles on a separate sketch and project so I can place them properly. But as far as I can tell the dog bones served there purpose. I have actually had this prototype cut on the CNC and the tabs/slots fit perfectly.

[davebYYPCU]

Start over or not, not sure that is any better / worse.

The origin is a bottom left.

The bottom left corner point of the right side tab, is horizontal to the Origin.

The bottom left corner point of the top tab is vertical above the origin.

To set them up, click on end points.

As for dogbones, you would make a second sketch, project points which would be centre points (lots of them) for the dog bones.

(Automatically fully constrained and no dimensions)

Finish sketch, make the plate, hide original sketch, make the dogbone centre sketch visible.

Start hole tool - set to sketch mode window select all centre points, set values and they are done in one step.

Check timeline.

[jcook27FELS3]

Okay. Going back through the sketch. Aligned the corners to the origin as you recommended. removing all the dog bones from the original sketch and then will use project for a supporting sketch containing the dog bone holes.

[jcook27FELS3]

I removed all dog bone circles as recommended, but before I create a sketch for the corner circles with a project, I need to get what I have constrained. I understand the constrain examples you guys have been showing, however the process is still hit and miss. Some things constrain and somethings don't and I get an over constrained error.

John H. - I have the inner wall example that you fully constrained loaded up (thanks). And I am trying to do the constraint operations on the original diagram to learn this - I don't understand why.

I am going thru and deleting old constrain symbols trying to get this to a point where I can start redoing things correctly. Also - I see in the previous example videos you select a line and pull it out of place demonstrating that it is not constrained 9because it moves). How are you doing this? When I click a (blue) line and pull on it it doesn't move? Is there a key I am supposed to holding down to move it?

Here are some unconstrained examples - what is the next step to constrain then. They are already dimensioned (not shown). The rectangle example is partially constrained. The other picture has atop horizontal line that won't take a constraint and a smaller horizontal line that also will not constrain. As far as I can tell I have correctly constrained the drawing to the origin as was suggested. You can see that in picture 3.