Another tolerance for Combine/Cut

[xeddog]

I have read a few other posts regarding creation of a tolerance between parts created using Combine/Cut, but the options do not work in this case.  At least by my greenhorn status.  I have created the spline shaft and base as shown in the attached screenshot.  The pieces are eventually going to be 3d printed so some clearance is a must.  I have printed the spline shaft, and several bases using a couple of things to get them to fit.  First was scaling which was a total bust because scaling alters some of the dimensions preventing the pieces from fitting at all.  Specifically, the inside wall of the splines in the base become too large. The holes in the corners would also be out of place, and wrong size.  I also tried creating an offset around the inner diameter of the splines, but that also fails because of the 45 degree taper in the sides about 1/2 way down.  So is there anything else to try other than re-designing the base and designing in the clearances in the dimensions?

Thanks,

Wayne

[mango.freund]

hello @xeddog   is this what you are trying?                   greetings mango

[xeddog]

Thanks for the reply, but not quite what I am after.  If the splines went all the way through the base as in your sample, I could use the outline tool and then extrude/cut as I have seen in other posts.  But I don't want the splines visible from the bottom and I have not found a way to maintain the tapered part so the splines do not go all the way through. 

I could redesign the base with a reduced thickness and let the splines go all the way through, sketch a new rectangle onto the bottom, extrude it out, cut a slightly larger taper, and then join the two halves.  

Bottom line - I was hoping for a more . . . "elegant" . . . solution that would allow me to keep the taper.

[jhackney1972 · Accepted solution]

I broke the link to the external file just to make a F3D file for easy of transmission, something you should do if you can before posting.  I used the Offset Surface command to generate the clearance amount, I used 0.25mm, but you can use anything you like.  Model is attached.

[xeddog]

The last sentence in your video - "Hope this helps."   YES IT DOES!!!  

One question (so far).   When you did your "crossing" to select all of the sides in the offset, You did indeed get all of the surfaces around the entire spline shaft.  When I did it, I only got the surfaces that were visible from my viewing angle.  I did not get the back side selected, nor any faces that I could not see.  I had to rotate the shaft on it's axis 90 degrees, ctl>cross three times to get all of the surfaces I needed.  Is this perhaps a limit in the hobbyist version, or a bug, a setting, or ???

Thank you very much

Wayne

[jhackney1972]

I also have a Fusion 360 personal license I use for testing.  The Crossing Window selection works the same in it as it does in the Subscription version.  Make sure you "cross" the complete model for what you want to select.  

By the way, when you post replies to a forum post, it is important that your select the Reply button on the post from the person you are responding to.  You, for example, selected a post written by you, so you get this screen capture below.  The reason this is important if you have more than one responder, which you do, no one knows who you are addressing your comments.

[jhackney1972]

Did the Crossing selection finally work for you?  Any other issues with the method?  If not, don't forget to mark your forum post as solved so others can find it if they have similar questions.

[xeddog]

I have attached an mp4 video of my screencast that shows the issue I am having with selecting using the crossing box.  I'm still working out how to post a link from my account. 
Anyway, It's like F360 doesn't realize that this is a body, but yet it is.  I tried using combine to make sure that all faces were a single body, and when I click on ANY face, the entire thing is selected like a body would be.  I can use move/copy as a body too.
Now the next thing.  After I get the shaft rotated and all parts selected,  I have a new body in my tree.  But when I attempt to do the Combine/Cut, I select the target body, but for the life of me I cannot select the newly created offset body as the tool.

[xeddog]

Here is a screencast of the next problem I am having.  After rotating the spline shaft and CTL>Box to get all of the faces selected, I finally get a good offset.  I then try to Combine>cut.  I select the square block as the Target, and then try to select the newly created offset as the tool.  I cannot select any part of the offset. 

[mango.freund]

hello @xeddog --- --- that's not a problem. look in the selection filters to see if there is a tick. why should the large bevel remain in the rectangular part at the bottom? that weakens the network and you cannot compensate.

what is wrong with my solution i gave?    greetings mango

[jhackney1972]

Two things, and I emphasis them in the Screencast.  First, check your selection filters and make sure they are all on.  We both use the same application so I know the Crossing Selection will work.  Second, you said you are trying to use the Combine command to remove part of the block body, that is the WRONG command.  You want to use Split Body and then remove the interior body from the block.  Watch the Screencast closely and it will work.  Your last Screencast did not show up on your post so I could not preview it.

[xeddog]

mango.freund - There is nothing *wrong* with your suggestion, and for THIS piece it would have worked.  But this is a decorative piece so strength isn't really too much of a consideration.  And, it was a good learning opportunity for future designs I might do.  I do appreciate your response, but it just seems like there had to be a better way.

[xeddog]

Thanks John, I finally got it through this thick skull of mine.  Here is what I I was doing wrong -
1.  Selection filters.  I did have "Select All" checked already, but what seems to have done the trick was checking "Select Through" at the top.
2.  The part where you re-activated the top level went right over my head and I missed that completely every time I watched your video.  Sheez!
3.  Same applies where you said to split body.  I had the Combine>cut on the brain and missed that too. 

I have marked your solution as ACCEPTED, and thank you very much for your knowledge and PATIENCE. 

[rickporter_]

Just came across this.  Exactly what I needed.  Thank you.