STEP Transform

[Chip Owner]

Chipster
I cut the job out on the only piece of stock that I had in the scrap bin, which was
full of holes before I started,  so didn’t post it before.
I didn’t think it would be of any use as my machine is a milling machine and my
spindle speed max is 1750 which limits the feedrates commensurate with the chipload
for the cutter.

The order of operations:
I drilled the holes first.
Then machined the pocket using a standard pocket mop, I’m a fan of the Troc mops but
for this one off job it wasn’t necessary.
Then I chamfered the holes.
Lastly I cut out the piece using a profile mop.

With the profile mop I didn’t use any holding tabs just left 0.25 mm up from the bottom of the stock and
 broke it free by pushing it out with my fingers, but if cutting it out as a real job would.

It’s a nice quick simple little job with no hidden gotcha’s.

If you're unsure about the speeds and feeds to use, sing out and supply the endmill details and
material spec and the max rpm of your spindle.

Dave
EDIT to add:
Chipster I just simulated the 3Dprofile file you provided earlier, with the same feeds and speeds
that I actually used when I cut the job out, it’ll take 27 times longer to cut out and the holes
won't be accurately positioned and won’t be round.

Lol  So in summary, I was making a mountain out of a mole hill!

Here's me plotting to make 2-3 different size vac beds to throw onto my large vac bed that is to big to hold down small parts and I hate double sided tape.  (I'm going to have to do this anyway, as I've been doing a lot of odds and sods on small cut offs of thin sheet lately).

Anyway, thanks for going this far and even cutting it.

I think my concern was the radius in the corner of the pocket transition and getting the radius right on the hole, it was written as 0.5mm radius.

I won't get it cut today, had a gig last night, 1st Christmas Party back at our former pre-covid pre-cnc business, as we don't do so many these days I always feel hungover the next day, even as a non drinker. I will look at playing with the mops you used, probably a lot faster too.

[dave benson]

and getting the radius right on the hole, it was written as 0.5mm radius.

For doing the radius or chamfer on the hole, you can use the Break Edges plugin
you can also put a small chamfer around the top face (called breaking the edges)
A chamfer at the bottom of the pocket requires that you make a copy of the pocket
level geometry (stick it on a new layer) so that you can work with it easily.
I’ve updated the Break Edges plugin and will put in the Break Edges thread.
I’ve also included the CB file as an example of the mop order, and put the required
geometry on separate layers.
If you want to use the plugin and find yourself struggling, then sing out and I’ll
give you some pointers, trips and tricks to use it.

Dave

[Chip Owner]

and getting the radius right on the hole, it was written as 0.5mm radius.

For doing the radius or chamfer on the hole, you can use the Break Edges plugin
you can also put a small chamfer around the top face (called breaking the edges)
A chamfer at the bottom of the pocket requires that you make a copy of the pocket
level geometry (stick it on a new layer) so that you can work with it easily.
I’ve updated the Break Edges plugin and will put in the Break Edges thread.
I’ve also included the CB file as an example of the mop order, and put the required
geometry on separate layers.
If you want to use the plugin and find yourself struggling, then sing out and I’ll
give you some pointers, trips and tricks to use it.

Dave

and amusingly I've just been trying to do this and indeed refresh memory on brake edges to soften the edges all round as you had done.

I tried convex radius in chamfer and didn't get anywhere on the circle.

[dave benson]

A few things to keep in mind.
When working with a model from 3D modelling software (I use Freecad) but the principles
are the same for all of them.

If you can roll back the timeline on your model to a point where the model has not had the chamfers
created yet, and export that.

If you don’t do this, then you lose the true Z position edge of the hole as when imported and
edge detected you get two polylines, the one on the top face is equal to the hole
diameter + 2 * the chamfer width, and the bottom polyline (which is the correct diameter) is
displaced in Z by the depth of the chamfer.

So you must select those polylines and raise them up to the surface Z height of the top polyline.
In the pic you can see the finished model and a rolled back model which is the one to export
as it will save you a ton of time and eliminate a lot of possible errors as you don’t have to adjust
the Z heights of the polylines.

Your 3D modelling software will have export settings for step files, If you step import doesn’t
work correctly, then in pic 2 are my settings used to export the step file.

Here for this model, I have un-checked “write out curves in parametric space of surface”
This simplifies the model and exports it as individual faces\lines.
For 3D printing I have this checked.

Another thing to keep in mind is that when the plugin starts up the default values give
a 1mm chamfer 1 mm up from the tip of the tool.

Starting to cut one mm up from the tip of the tool is the bare minimum and I use 2 mm, this
is so that I don’t break the tip off the tool and the further up the tools cutting face you
start cutting, gives a better finish, because the actual surface cutting speed will be higher.

The other thing is you can use all of the length of cutting edge, as the tool wears.

Dave

[Chip Owner]

A lot to take in there as a newbie to this 3d stuff. Only recently managed to sort the graphics on laptop out to be able to start playing.

Useful stuff, I think the 1mm might be too aggresive for this part, so might be I have to resort to hand deburr tool.

I did start to play today, I pushed my luck on the holes with a 3mm bit. The only larger bits I had were 8 & 9mm high speed steel remnans from when I used to slot and keyhole profile with a handheld router. I didn't want to use them and instead of doing a rough pocket with the 3mm or drill mop I thought I could get away with a shallow, slower profile cut, until the bit broke.

I'll have to cut another length off the bar stock and have another go, tomorrow I'm back on plastic so may not get chance then.

[Chip Owner]

Not as clean as I'd like but succeeded in the milling.

Stupidly added some positive clearance on the lower part pocket trying to clear it with an 8mm tool when I should have reverted to the 3mm and couldn't do the chamfer edge as all my v bits were to big to get round the lower part.

My take home from it at least as far as this drawing and part is it didn't need a step file, a DXF would have done on this occasion, I spent more time worrying if I'd got the file right when I should have been focussed on the cutting operation.

It was a useful exercise though.

[dave benson]

Stupidly added some positive clearance on the lower part pocket trying to clear it with an 8mm tool when
 I should have reverted to the 3mm and couldn't do the chamfer edge as all my v bits were to big to get
 round the lower part.

It looks good, there is a property in the side panel called cut width, where you can cut wider
than the width of the tool, I used this to clear out some extra material for clearance for reasons.
For example If you use a  6 mm tool but set the cut width to 8 mm then you would get an 8 mm
wide cut.
The cut width property is not the same as a roughing clearance property where you want to cut
or leave a little extra material.

Dave

[Chip Owner]

Stupidly added some positive clearance on the lower part pocket trying to clear it with an 8mm tool when
 I should have reverted to the 3mm and couldn't do the chamfer edge as all my v bits were to big to get
 round the lower part.

It looks good, there is a property in the side panel called cut width, where you can cut wider
than the width of the tool, I used this to clear out some extra material for clearance for reasons.
For example If you use a  6 mm tool but set the cut width to 8 mm then you would get an 8 mm
wide cut.
The cut width property is not the same as a roughing clearance property where you want to cut
or leave a little extra material.

Dave

Now that is interesting, I need to play with that it could come in handy.

I was in the end in a hurry between paid jobs to get this done just to confirm I had fully understood the step file process.  I've just run caliper over it and it is out, but can see where this happened.

This is what I'm finding, I've cut sheet stuff (99.9% thin alu) using the settings for so long, understanding the broader scope of what the software can do escaped me also learning what my machine can do.

Looking at this from a commercial perspective as a type of machining itself, (which is what so far has stopped me finishing any arty 3d carves),  in this instance, despite making a fixture plate some time ago to test something like this, the set up took as long as the cut if not longer, I'm not sure it's anything I'm ever likely to develop.

I have some ideas to make smaller vacuum beds that I can lift on an off my main bed and use as required for small parts, perhaps as an when I get this done, if they perform, I may play more.