Using Tabs - Sanity Check

[richardsalzman]

I have a good-sized piece of .375 thick 6061 aluminum.  I plan on cutting out a bunch of shapes and use the tab function to created tabs that I will later trim away.  This is the first time I am using this tab feature.    I used the following setting to size the tabs.  Just curious if these look like they make sense?

Thanks... Richard

[jeffescott]

I use the fusion recommended triangular tabs sizes for 6061 extrusions.   I manually select locations of tabs,  based on support and the ease of removal.  

[DarthBane55]

Looks good to me.  Probably too many tabs, you'll find them to be fairly strong still, specially at 0.060" thick.  We usually make them about 0.030" thick and use 2 per edges only.  We do prefer the rectangular ones like what you did, but this is going to be personal preference, just try and see.  You have to experiment a little bit and will quickly find what works best for you.

[programming2C78B]

Depending on how you plan to remove them, I'd rather side on having too many and adapting your rule of thumb as you keep making things. 

We like .02" thick tabs, about 3/4" wide when tabbing off parts on the 5th axis. 

[richardsalzman]

Thanks for all those tips.  Very helpful.  One last question on this project.  These pieces are going to fit into a hub (see below).  I want as tight of a fit as possible.  Currently, I am using a 2D contour to cut the profile of these.  I have two finishing passes at .010 inches.  Do you think it is worthwhile to add a repeat finishing pass so that all of these parts have minimal size variation and allow me to machine the hub to tightly fit the wings?

[DarthBane55]

Yes, it would remove the small taper that the 1st pass might have left.  More importantly, you should set compensation to "wear" so that you can adjust the diameter offset in the machine.  If you make the blue parts 1st (I would since you have so many of them done all at the same time), when you get to the hub, adjust your diameter offset to cut smaller than wanted and gradually adjust the size until you get the fit you are after.  Do this with the 1st pocket only, once the DOFF is set the rest should all be the same size, providing you got a decent machine.

[richardsalzman]

Thanks!  I was going to approach this and use stock to leave in place of the "wear" feature.  I never used wear before but will give it a try.  Thank you!

[programming2C78B]

Wear is only available on some machine controllers. I'd just make the pocket +.003" to start and you should be ok. 

[richardsalzman]

Yes.  That is what I had in mind, I was just questioning if I should do the repeat finishing pass when machining the profile.  Looking like that will produce a more consistent dimension across all of the parts.

[DarthBane55]

Yeah, wear is only available on some machine controllers.  If his machine has it, he should use it.  If it does not, he can't.  Pretty simple. And he should start with pocket at -0.003 and gradually go up for the fit he's after.  If he goes +0.003 it is not a slide fit (which is what he was after I think).

[programming2C78B]

I only use Repeat Finish when aiming for tolerances below .001" 
I don't like the idea of intentionally rubbing an endmill along a part when the better/my practice is just making sure the finish pass isn't so wide/heavy it causes so much deflection that it causes an issue with fitment.

If you cut those fins at 1" and a programed 1.003" pocket everything should fit together quite nice right off the machine. There will be some deflection/wear/undersize on both cuts that make for a real nice fit. 

[DarthBane55 · Accepted solution]

ok you win Master, I will try not to post any advice when you do because you are correct every single time, other people's inputs are just interference in your perfect methods, I apologize for trying to help when obviously they should only listen to your advice, my bad.

This is why I was out of this forum for a long time, I will go back to that, works better for my mental health.

[richardsalzman]

Hey guys, machining is both an art and a science.  I am a hobbyist with absolutely no real machining experience and have learned a boat load on this forum by looking at this stuff from many different points of view.  I learned so much on from guys on this forum that I sold my benchtop converted mill and recently bought a small vertical machining center.  Darth... keep your ideas coming!  This forum is all about learning from everyone.  

Perhaps I did not explain my question well.  This part consists of "wings" that fit into a hub with M4 screws that hold the wings to the hub.   I don't have the knowledge to provide details on actual tolerance for fit, but my goal is to have the wings fit snuggly into the hub so that the tight fit helps to hold the wing in place and minimizes lateral movement.  This will minimize the load on the M4 screw.  

My question is if I don't use a repeat finishing pass, and the 1/4" end mill flexes slightly while cutting the profile of the wings, will all the wings be the same size and will the end mill flex the same throughout all the wings or will I get a tighter tolerance and will the wings be closer in size to one another if I use the repeat finishing pass.  If all the wings are as close as possible in size to one another, then I can machine the hub to fit the wings tighter.  I'm sure this is all over-kill, but this it is how I learn for the next more demanding project.  

Thanks again for all your thoughts... and I mean ALL your thoughts😊

Richard

[lauri_barnhart]

Hi @richardsalzman, thank you for your question.

Did the responses provided by @jeffescott, @DarthBane55 or @programming2C78B help answer your question?

If yes, feel free to click on the Accept Solution button.

This helps other users benefit from the information.

In case you still need help, please provide an update here so we can help you best moving forward.

Thanks!

Lauri | Community Manager