Hit a snag again :)

[precisionmetal]

I think my approach would be to machine as much of this part as possible from one side. Note the corner with green arrow (and the opposite side as well) will need to have a fillet at least as large as the radius of your cutter.

Once I've gone as deep as possible and completely finished the top side, I'd add maybe 4 tapped holes where the red arrows are. Then I would bolt the part to a rectangular plate of material by those 4 holes, and flip it over (hold by the bolted on plate), and finish the back side.

Yes... your part will have 4 tapped holes in it, but those could just be drilled and chamfered in a drill press and made to look like a "weight reduction feature".



PM

[daniellyall]

Dave here's one way to do it so the tabs line up for both side A360

All it is duplicating the first setup with it's toolpaths then flipping the Z axis in the setup and moving the bottom height to stock bottom for all toolpaths and changing the 2D profile back outside.

I added the patchies to allow the adaptive to cut down to the faces on the first side and the sketch for the 2D profile toolpath so you can guarantee the tabs are going to line up on the second side.

How to have the flip and line up done that's up to you but I would have the stock modeled and drill a couple of holes in it and use one of the holes for the WCS for both setups this works well as long as the holes a straight.

[precisionmetal]

Interesting approach Daniel. I have never used tabs yet... but now see how it's done.

Thanks for posting that!

[davek0974]

Just to be a smartass
Attachment 386866

Nobody likes a smart-arse, well maybe i do this time, very nice, that is what i envisioned myself

[precisionmetal]

I'm "guessing" that he might have left the "flange" large.... applied the fillet, then trimmed the flange?

PM

[davek0974]

Thanks guys, i'm going to have another play with this later today.

I really can't drill / tap it, needs to be a smooth finish really, I'll explore further with the "router" method as that makes sense to me, see how far we get.

[daniellyall]

Put the hole in a spot that's going to be cut out in the last setup you have enough surfaces area that's going to be completely removed in the last op that you could stick a few dowels in it to use as the WCS.

In fusion the WCS can be wherever you wont it to be, you can even change it if you lose power and have to rehome the machine, it's up to you not the cam program, just have a look at what I added to your model to make it easier to cut some parts that's just 2 off the many things you can do to make it easy as mud.

[davek0974]

I'm having no luck at all with this - I can't seem to get a selection that goes where i want, the web link posted below by daniellyall keeps crashing my browser and i've spent way too many hours on it and got nowhere

One of those days, jobs etc.

I'm forgetting about the chamfers at present, they just add to the lack of knowledge i think, added complications not needed. Tonights idea was to hog out the hole plus the waste between the jaws, the hole was easy but selecting contours for the jaw gap just seemed to ignore the jaws and machine them off level with the opening behind, no idea why but it consumed a few hours figuring out that i had no idea why it did that

I guess it may be easier to forget the router method and go the fixture way, possibly, even if it means drilling holes in it. That way i could likely just throw a 3d path at the whole part and have at it, will see if that honours all the profiles....

[precisionmetal]

Try creating a sketch (which will all be on a single plane), and use the sketch geometry (rather than the solid model edges) to define the tool path inside that jaw gap.

[davek0974]

Will try that, thanks

In fact, since ditching the method i wanted and just letting a 3d adaptive go at it, it seems better, just means i have to figure in fixturing on side 2.

I will try the sketch method though now.

[precisionmetal]

Dave,

Many different methods to do the opposite side. Some depends on if you are making only one part, or maybe a few?

If you put another piece of material down on the table next to your part, you could cut 2 "islands" onto it which would lock your part in x/y position. You could clamp near the outer edge, and cut the inside of the part, then tap a hole in each island and make/use a clamp to hold the part down from inside the islands to finish the outer portion.

Off the top of my head, I can't think of a simple way to finish the back side in a single cut. Whether you cut away tabs, or cut inside/outside, or whatever you do... you may be stuck with multiple cuts on back side unless you cut a set of soft jaws to hold the part.

PM

[davek0974]

Moving forwards now, at last.

Got the first side cam'ed

I have opted to machine the whole surface of the front, its more time but i was hoping to machine down to mid-point, finish-pass the front, then flip over and mount in the vise with the new face as bottom Z in the step-jaws. Now i might be able to work the back as a mixture of full-face plus contour passes with tabs, something like that anyway

I programmed in a machined reference for X axis, z will be the new mid-point and y will be the opposite vise jaw.

Possibly

[davek0974]

This part is killing me

Never had so much difficulty getting near what i want!

Got the front making sense, i machined a face, full depth in the middle of the left edge so i could use it as a reference point for Xref on the flip-side.

Now, i thought i saw a video where there was job with multiple or split ref points - so i could pick the machined edge as my Xref, the top of the vise jaw as my Zref and the side of the vise jaw as my Yref

Think i could figure out how?

Nope

Is it even possibe???

[precisionmetal]

All possible, though you may need to add or subtract a measured amount from one or more of those touch-off points.

If I flip a part after one side is machined, I almost always end up choosing whatever face the part is resting against (step jaw, table, fixture) as the Z0 for my 2nd op.

If you are choosing the face of a vise jaw as Y0, simply choose your box point as one on that edge. If there is none available, just create a sketch on the face you'll be selecting, and draw a 'point' at the exact location you want to use as Y0. Then show the sketch in CAM, and select that point instead of one of the stock box points.

Hope that helps...

PM

[davek0974]

Getting there, thanks.

Story so far...

Setup1, top side, machine to finish size down to mid-depth, chamfer edges. Stock is machined over the whole face.

Setup2, underside, machine to finish size down to mid-depth +1mm, chamfer edges. Stock is machined to a boundary box leaving 10mm for the vise jaws.

In my mind i should now have a finished part held in the stock by a 1mm web all round. This is then removed, leaving tabs with a smaller tool.

In theory it might work, my main concern is that there is not enough waste on the ends of the test piece of stock to withstand the vise pressure and it will collapse when the web is cut. Later models i can leave more stock, a bit wasteful but will save time.

[daniellyall]

Make the tabs bigger and use some super glue or double sided tape on the vise jaws then when you do the second op have it just held in the vice jaws, the super glue or double sided tape will do all the holding.

[davek0974]

Just about ready to bin this part and give up!!

After days and days of messing with paths and strategies, dropping features i wanted etc, I finally get a recipe that might actually work, no warnings in CAM and what happens?

It will not post - just get the .failed extension.

Its failing on the chamfer op of front and back side despite simulating nicely.

Hers a link...
A360

I just do not know why this seemingly simple part is so hard, or is it hard and i'm just thinking it should be simple?

Not much point if it won't post anyways

[daniellyall]

It posted fine for me what post are you useing

[davek0974]

One that i have been using since i started - Mach3Mill IIRC

[davek0974]

The error in the log is

"Error: Failed to invoke function 'onSection'."

No idea why.

The post was edited some time ago by Fusion support to alter the code for rigid tapping on my mill, I have also edited a line so that it outputs G43 H0 for every tool as my mill does not use tool length comp and it would cause issues.