What type of clearance for a sliding lid box

adam_dezolt_

Hi. I'm brand new to cad and have been playing around with the onshape app and was wondering if anyone could offer any advice. I'm trying to design a simple sliding lid box to be milled from aluminum. What type of fit is the lid to the box (I know I don't want an interference fit) and how much size difference should there be between the too? This is just a basic attempt with the app plan on starting over once I get a better hang of things. I'd hate to send out a design to cnc for the first time and realize I'd overlooked somethinig.
Again any advice would be awesome.

Thanks you in advance 
Adam

_Ðave_

Adam, Depending on how the lid will be locked in place. If the lid is staying closed by the friction of the fit than the fit will have to be very close and expensive to machine.

 If the lid is locked closed by some sort of spring plungers inserted into the two holes than you can have much more clearance and reduce the cost of machining.

 basically the more clearance you can allow than the more tolerance you can allow the machinist and reduce your machining cost.

 Also the fillet radii looks awful small relative to the depth of the pocket.

 You'll need to provide a bit more info for someone to give you a reasonable answer.   

coleman

@adam_dezolt_  I engineer and make (cnc) caddys just like this one for a living in the medical instrument industry.  

Couple of things
1) You should probably consider increasing the radius in the corners of the pocket.  While it is impossible to guess dimensions from your model...the radius looks small in relation to the depth of the pocket.  When machining that pocket a cylindrical cutter is used that will leave a radius in the corners.  We want to use a larger diameter cutter for a deep pocket like this one.  Also, make the radius about .01in bigger than a standard dimension for improved surface finish.  For example: if you can bump the radius up to 3/8....make it .385 as opposed to .375in.  I can provide more information as to why if you want me to.  

2)  I recommend adding a ball plunger to retain the lid on the caddy if possible. You can either do a press fit plunger with a flange or a threaded plunger.  Press fit with flange is best in my opinion for this particular application.

3) Will the aluminum be anodized?  Both the caddy and the lid?  If so you will need to account for the anodizing thickness.  

4) Your current design will allow for a nice flush look between the lid and the edge of the caddy.  This is fine if it is absolutely required.  You might be better off with a completely planer lid with no cut outs on the sides, and let the 3 perimeter edges of the lid slide under the lip on the caddy.  Again I can go into more detail if you want me to. 
These changes will make the caddy and lid more cost effective to machine.  

In regards to tolerance, it is difficult to say without knowing how you plan to retain the lid on the caddy.  A purely friction fit will be tough and more expensive to produce- quite frankly the friction fit lids in aluminum are a pain to remove.  Aluminum is a gummy material.  

Also, what are the overall basic dimensions?  How long, wide and deep is the caddy?  How thick is the lid?

michael3424

Could galling be a problem for this box?  I've seen that happen with aluminum parts that slide across each other.

adam_dezolt_

michael3424 said:

Could galling be a problem for this box?  I've seen that happen with aluminum parts that slide across each other.

I did not consider galling. I'll have to plan around it
Thank you

_Ðave_

Magnets are a good concept. .003 clearance @ maximum material condition should be fine. If the slot and lid both have +/- .002 tolerance than your clearance would be between .003 and .011. which is reasonable and won't have an issue with galling unless the parts get nicked and damaged. anodize would help with that but than you'll have to allow for plating thickness.

adam_dezolt_

Oh I just looked at my screenshot and realized I should have modified the top portion of the lid to fit proper before posting sorry

_Ðave_

Adam, Depending on how the lid will be locked in place. If the lid is staying closed by the friction of the fit than the fit will have to be very close and expensive to machine.

 If the lid is locked closed by some sort of spring plungers inserted into the two holes than you can have much more clearance and reduce the cost of machining.

 basically the more clearance you can allow than the more tolerance you can allow the machinist and reduce your machining cost.

 Also the fillet radii looks awful small relative to the depth of the pocket.

 You'll need to provide a bit more info for someone to give you a reasonable answer.   

coleman

@adam_dezolt_  I engineer and make (cnc) caddys just like this one for a living in the medical instrument industry.  

Couple of things
1) You should probably consider increasing the radius in the corners of the pocket.  While it is impossible to guess dimensions from your model...the radius looks small in relation to the depth of the pocket.  When machining that pocket a cylindrical cutter is used that will leave a radius in the corners.  We want to use a larger diameter cutter for a deep pocket like this one.  Also, make the radius about .01in bigger than a standard dimension for improved surface finish.  For example: if you can bump the radius up to 3/8....make it .385 as opposed to .375in.  I can provide more information as to why if you want me to.  

2)  I recommend adding a ball plunger to retain the lid on the caddy if possible. You can either do a press fit plunger with a flange or a threaded plunger.  Press fit with flange is best in my opinion for this particular application.

3) Will the aluminum be anodized?  Both the caddy and the lid?  If so you will need to account for the anodizing thickness.  

4) Your current design will allow for a nice flush look between the lid and the edge of the caddy.  This is fine if it is absolutely required.  You might be better off with a completely planer lid with no cut outs on the sides, and let the 3 perimeter edges of the lid slide under the lip on the caddy.  Again I can go into more detail if you want me to. 
These changes will make the caddy and lid more cost effective to machine.  

In regards to tolerance, it is difficult to say without knowing how you plan to retain the lid on the caddy.  A purely friction fit will be tough and more expensive to produce- quite frankly the friction fit lids in aluminum are a pain to remove.  Aluminum is a gummy material.  

Also, what are the overall basic dimensions?  How long, wide and deep is the caddy?  How thick is the lid?

michael3424

Could galling be a problem for this box?  I've seen that happen with aluminum parts that slide across each other.

adam_dezolt_

coleman said:

@adam_dezolt_  I engineer and make (cnc) caddys just like this one for a living in the medical instrument industry.  

Couple of things
1) You should probably consider increasing the radius in the corners of the pocket.  While it is impossible to guess dimensions from your model...the radius looks small in relation to the depth of the pocket.  When machining that pocket a cylindrical cutter is used that will leave a radius in the corners.  We want to use a larger diameter cutter for a deep pocket like this one.  Also, make the radius about .01in bigger than a standard dimension for improved surface finish.  For example: if you can bump the radius up to 3/8....make it .385 as opposed to .375in.  I can provide more information as to why if you want me to.  

2)  I recommend adding a ball plunger to retain the lid on the caddy if possible. You can either do a press fit plunger with a flange or a threaded plunger.  Press fit with flange is best in my opinion for this particular application.

3) Will the aluminum be anodized?  Both the caddy and the lid?  If so you will need to account for the anodizing thickness.  

4) Your current design will allow for a nice flush look between the lid and the edge of the caddy.  This is fine if it is absolutely required.  You might be better off with a completely planer lid with no cut outs on the sides, and let the 3 perimeter edges of the lid slide under the lip on the caddy.  Again I can go into more detail if you want me to. 
These changes will make the caddy and lid more cost effective to machine.  

In regards to tolerance, it is difficult to say without knowing how you plan to retain the lid on the caddy.  A purely friction fit will be tough and more expensive to produce- quite frankly the friction fit lids in aluminum are a pain to remove.  Aluminum is a gummy material.  

Also, what are the overall basic dimensions?  How long, wide and deep is the caddy?  How thick is the lid?

Wow! First thank you for being so thorough this is very helpful.

I'm planning to use the box as housing for a vaping device. It will have to have a rc style li-po battery (I plan on having vent holes in the case to prevent total catastrophe) , a chip for regulating voltage, 3 switches and wiring. 

Until I purchase the battery and have one in hand to measure  (I've heard rc type li-po can vary 2mm or better) and leave room for wire and battery expansion. The inside dimensions  will probably end up around 6"L x 1.5"D x 3.5"W. And about 1/4 to 3/8" wall thickness. Not 100% though on the wall still learning what's possible vs my ideas

My thinking with the holes was using neodymium magnets that line up with holes/magnets on the back side of the lid. Only because I have a bunch in my tool box. The only thing I can see go wrong would be, if adhesive gave way and one of the pairs shifted. Where one magnet was in both the lid and box at the same time.

The radius of the cutter is something that I should have  thought of. I'll definitely go .01 larger than standard.

I am leaning towards a flush fit lid. However a simple lid set in to the box as you suggested will simplify things greatly. that may be the way I end up going.

How do you think the magnets  will preform as a closure? Do you know of any websites with more information I could learn from?

Thank you for your time 
Adam

adam_dezolt_

michael3424 said:

Could galling be a problem for this box?  I've seen that happen with aluminum parts that slide across each other.

I did not consider galling. I'll have to plan around it
Thank you

adam_dezolt_

_Dave_ said:

Adam, Depending on how the lid will be locked in place. If the lid is staying closed by the friction of the fit than the fit will have to be very close and expensive to machine.

 If the lid is locked closed by some sort of spring plungers inserted into the two holes than you can have much more clearance and reduce the cost of machining.

 basically the more clearance you can allow than the more tolerance you can allow the machinist and reduce your machining cost.

 Also the fillet radii looks awful small relative to the depth of the pocket.

 You'll need to provide a bit more info for someone to give you a reasonable answer.   

Hi thanks The fillet will be sized .01 larger than a standard bit as Colman mentioned. Definitely somthing I would have overlooked. I was thinking of using the holes for magnets that line up with another pair of magnets in the lid ( just cause a have bunch). What are your thoughts on magnets as a closure? I think I'm going to simplify my next attempt to keep cost down.
Thank you for your input 
Adam

_Ðave_

Magnets are a good concept. .003 clearance @ maximum material condition should be fine. If the slot and lid both have +/- .002 tolerance than your clearance would be between .003 and .011. which is reasonable and won't have an issue with galling unless the parts get nicked and damaged. anodize would help with that but than you'll have to allow for plating thickness.

adam_dezolt_

Hey thanks alot Dave. I'll definitely use that tolerance in My final design. Not sure about anodize yet as that's gonna depend on cost.
All these answers are incredibly helpful I'll probably learn alot just reading on these forums

Adam