Very Thin Floor

[Metals and materials]

Curious and wanted to broaden my perspective in machining thin floors. Issue is the floor thickness being too thin. I am using scallop to clean the floor. Attaching the parts here, any advice/recommendations are appreciated. Thank you! 

In pic, you will see the floor is going point like surface. When machining, it torns that part apart. I am using two contours on side to clean (the side). 

 

Attaching different angular pics here. 

[JParis]

That floor should be supported and "if" it can be fixtured flat, I would attempt 2 passes with a reverse flute spiral endmill

 

[CEMENTHEAD]

imho, small depth of cuts, small tool, don't be greedy. thin parts take time. 

[Aaron Eberhard]

Don't forget that Dynamic roughing can really be used effectively to control the amount of stress put into the part.  If you use HSM advisor or equivalent, play with the stepover numbers until you get a minimum of cutting force, and leave just enough for a skim pass if you would prefer a different finish on the floor. 

Take that with both of pieces of advice above, small tools impart less cutting force than large ones, and I've used double-sided tape under thin floor areas to help squash vibration.

Stress-relief is a good idea if it's a high tolerance thing, rough it out, release all clamps, secure it for finish pass.

It's hard to give more specific feedback without knowing materials, sizes, tolerances, etc. 

[JParis]

1 hour ago, JParis said:

That floor should be supported and "if" it can be fixtured flat, I would attempt 2 passes with a reverse flute spiral endmill

 

That should have stated 2 passes "after roughing"  CEMENTHEAD is right, can't rough to hard or too much

[Metals and materials]

@JParis@Aaron Eberhard @CEMENTHEAD 

Floor Fixture support, good idea. I can make fixture angled to what the part is. 

I am going slow but I will use endmill with small diameter. 

Unfortunately, I do not have HSM Advisor. But now I am gonna take a look at it. I will give your reference @Aaron Eberhard lol. I will ask for some extra discounts as well!

Okay, so I was roughing 0.002 above the surface. I will increase that to 0.005 or something and then finish little by little. 

[Aaron Eberhard]

33 minutes ago, Metals and materials said:

@JParis@Aaron Eberhard @CEMENTHEAD 

Floor Fixture support, good idea. I can make fixture angled to what the part is. 

I am going slow but I will use endmill with small diameter. 

Unfortunately, I do not have HSM Advisor. But now I am gonna take a look at it. I will give your reference @Aaron Eberhard lol. I will ask for some extra discounts as well!

Okay, so I was roughing 0.002 above the surface. I will increase that to 0.005 or something and then finish little by little. 

 

I promise that you will save more in than the $195 lifetime price on in the first month in cycle time & tool life if you're programming every day.  Every month after that is pure profit.  It's awesome.  It was one of the first purchases I made when heading out on my own.  It lets me start from VERY good feeds and speeds in pretty much every situation.   Eldar is awesome, tell him I said hi

For example, let's say this part is 6061-T6, and you're trying to figure out how different roughing strategies would work on this part.   Let's assume that you're cutting a .5"thick piece down to leave a .075 floor (removing .425").  Remember that we have no clue what the real sizes of the part are

For a .375" 3FL Endmill w/ .625LOC and .75" Stickout, in full attack mode (100%), HSM advisor recommends 63.3% stepover (.2373) for a Dynamic path, 102.73 IPM/13409RPM (.00255 FPT, 1316SFM).    It doesn't know that it's thin-floor, of course, but it says that it will be putting 66 lb of cutting force into it (using 2.6HP).   Now, we know that's way too much, if you took the part out and applied 66lb of force there, you'd bend it quickly.

Taking the same exact everything with a .25" Endmill recommends a 31.6% stepover (.079"), 133.5IPM/23798RPM, which = 24lb of force.   Getting closer! 50% of feed & speed equals 12.1 lb of force, etc.  

No matter you scale it, a .25 endmill is putting a lot of force into something you can probably bend with 2 to 3 lb of pressure, right?

A .125" Endmill goes to 5.4% (.0068), 559IPM/98147RPM which would equal 4.2lb.    Now, my machine won't go to 98k!  So if I type in my max in this scenario, let's say 10,000 RPM, which is 10% of its recommended value for this cut, that slows it down to 5.7IPM, but it's only putting .42 lb of force into the cut.    That could work!

[Leon82]

Tabs on both sides. Then chop off after the floor is done

[Metals and materials]

16 hours ago, Aaron Eberhard said:

Eldar is awesome, tell him I said hi

For Sure!!! 

 

16 hours ago, Aaron Eberhard said:

but it's only putting .42 lb of force into the cut

Ok wow interesting. I can visualize now.

[TFarrell9]

17 hours ago, Aaron Eberhard said:

 

I promise that you will save more in than the $195 lifetime price on in the first month in cycle time & tool life if you're programming every day.  Every month after that is pure profit.  It's awesome.  It was one of the first purchases I made when heading out on my own.  It lets me start from VERY good feeds and speeds in pretty much every situation.   Eldar is awesome, tell him I said hi

For example, let's say this part is 6061-T6, and you're trying to figure out how different roughing strategies would work on this part.   Let's assume that you're cutting a .5"thick piece down to leave a .075 floor (removing .425").  Remember that we have no clue what the real sizes of the part are

For a .375" 3FL Endmill w/ .625LOC and .75" Stickout, in full attack mode (100%), HSM advisor recommends 63.3% stepover (.2373) for a Dynamic path, 102.73 IPM/13409RPM (.00255 FPT, 1316SFM).    It doesn't know that it's thin-floor, of course, but it says that it will be putting 66 lb of cutting force into it (using 2.6HP).   Now, we know that's way too much, if you took the part out and applied 66lb of force there, you'd bend it quickly.

Taking the same exact everything with a .25" Endmill recommends a 31.6% stepover (.079"), 133.5IPM/23798RPM, which = 24lb of force.   Getting closer! 50% of feed & speed equals 12.1 lb of force, etc.  

No matter you scale it, a .25 endmill is putting a lot of force into something you can probably bend with 2 to 3 lb of pressure, right?

A .125" Endmill goes to 5.4% (.0068), 559IPM/98147RPM which would equal 4.2lb.    Now, my machine won't go to 98k!  So if I type in my max in this scenario, let's say 10,000 RPM, which is 10% of its recommended value for this cut, that slows it down to 5.7IPM, but it's only putting .42 lb of force into the cut.    That could work!

Thanks for giving some examples, I hadn't realized it had those kinds of calculations. That's really cool.

Can the Mastercam tool libraries be imported into the software? That's kind of how I read it on their website. 

[Aaron Eberhard]

1 hour ago, TFarrell9 said:

Thanks for giving some examples, I hadn't realized it had those kinds of calculations. That's really cool.

Can the Mastercam tool libraries be imported into the software? That's kind of how I read it on their website. 

You're welcome

It can go back and forth (I think he has some videos up on how it works), but I honestly don't use it much..  In my case, I can manage everything I want via Mastercam, so I just use the desktop version and enter values as appropriate into the toolpaths.   This is a prime example of where you might have the same tool but specific settings (stepover/DOC/etc.) for this one toolpath.