HSM/3d Milling Advice

[pinguS]

Hi all

I have attached a pdf picture of a part I make out of a 42mm turned billet.

It is quite basic, 42mm square at the bottom, going up 10mm at an angle of 30deg (60 deg depending which way you look at it). The bottom end has 5mm radius's going upto sharp points. This is just caused by the convex cutting action.

Currently I machine this quite simply with a 60deg cutter at full depth and let the machine get on with it (3 axis machine), with a simple program again as another post of mine:
x-
x+ r5.
y- r5.
x- r5. etc etc

My question is, if I wanted to use a ball nose cutter, which method would be best, 2D profile with wall draft angle set or the HSM option, or any other better method?

I know people say, why change something that works, but I'm looking at the speed factor and cutter availablity, as I find ball nose cutters quicker than angled ones, also if I wanted to change the angle, then buying a new cutter everytime is a head ache.

Can somebody please advise, and please take a screen shot if you recommend a HSM method or 3d milling, as that option is still mysterious to me. I could use the 4/5 axis machine, but thats to easy, and wish to learn a form of pencil milling on the 3 axis. I have tried the wall draft angle, but never got it to work right, the corners just ballooned out, so must be something I'm missing. I would prefer just to do this with one cutter, oh yes this is an aluminium part

Remember, speed is something I and probably everyone is after, then tweak the quality.

[dengo]

Here is a Helical Toolpath that would do the trick.
One entry and one exit. Very neat and tidy.

These are all the default settings in the toolpath so there is no need to think HSM is too complex for a simple op.
I have found that this type of op works very well as a 2.5 alternative for more complex profiles.

Obviously this is the finish op and assuming the roughing is done.

Keep plugging away.

[pinguS]

Looking at the attachment, would this kind of step down give a clean finish, or would it need to be increased? The attachment looks as if it would be a "record" type finish, or is it for display purposes only?

[mattpatt]

Dengo's choice of helical HSM is a good one.

Surface finish is basically down to how long you want to spend on the part.

I just had a quick look and finishing with the (default) 6mm ball nose, using adaptive stepdown with scallop set to 0.025mm, I reckon you'd get a nice looking finish.

It'd just take a lot longer to machine than you'd probably bargain for.

I did some similar parts for a mold not too long ago. Dengo gave me some advice then using helical HSM. The parts cam out great. They were used in an epoxy mold for a Yamaha R1 front fender. Finish was very good and just needed a bit of a buff before being used.

[pinguS]

Ok, with the standard setting on this part, I shall see how long it takes, but is the solid verify a good representation of what to expect or, does Solidcam over exaggerate on the computer screen?

[pinguS]

hey dengo, I tried the HSM with standard settings. Helical strategy.

I have played around with it, but could not get the cutter to go beyond the bottom of the part. i.e. the depth of the part is 10mm, so the ball nose cutter only down to 10mm, but as it is ball nosed, i was expecting it to carry on for another 3mm, (6mm ball nose default), to -13mm.

Currently, when I look at solid veriify, the bottom of the part looks like the end of a slide.

Have I missed a setting?

Also I am assuming that the contraint boundaries are just to control where the tool can go, but on this part there is nothing it can possibly hit, even on the machine, can I not have "no" contraint boundaries?

I have the hsm manual, boy is this long and I can't seem to figure this one out..

cheers for the advice...

I have just noticed the when I output the gcode for the above 6mm ball nose cutter, the arcs are in segments of x and y, I would have thought it would be the same for the output I get using a profile operation with g2 and g3. I have messed about with the mac file, and wondering whether I have disabled it there, or is this a characteristic of high speed machining? This is the same even if I use constant Z HSM...hmmmm
I have asked this question in thread "HSM Constant Z profile - G Code " link HSM Constant Z profile - G Code

[dengo]

Hey PinguS,

To Get the toolpath to extent past the bottom of the tool try increasing the Offset Value in the Tool on working area box. I have set it to "External with +3mm" offset for the example. Set Z bottom in the passes to allow for the Tool rad, so in our case it will now be -13mm.
That should now machine all the way down to the bottom edge.
I don't normally use the "No" constraint boundaries and can't think of one of my parts that I'd use it for unless by accident.

I think Solidverify is giving you a pretty good idea of what the finish is going to be like but again on the example that is a 0.5mm/full revolution step-down so its going to leave a bigger cusp height than you'd probably want.
Also the example didn't have the correct feeds and speeds so when you pump those in its a pretty quick op.
In this case you can't get it any quicker because there are no air move at all apart from ramping in and out of the job at the start and end of the toolpath.

And as for the G01 vs. G02 in the post..!%*$@, I gave up on it. I never got an answer from Solidcam that made any real sense to me but I think it has something to do with the algorithms that calculates the toolpath. Way over my head.

And the HSM book, you should see the 5 axis one I have on my desk !!!

The best advice I can give you is stick with it because I think its so much better than 3D for stability. All I have done is to just be strict with myself and try to get a toolpath even if I knew I could do it in 3D just to see what it looks like.
Just do yourself a simple part and play around with the options. The hardest thing is knowing what you can ignore with those thousands of options.
Links and leads are a classic.
What rad should I use? what angle? how long should the leads be?
Set them all to zero.
You'll still get a great looking toolpath without all the swirly bits that you probably don't need for most jobs. I know I don't !!!

Hope it all helps and sorry for the GIGANTIC post guys

[jamesu229]

I would suggest 3 axis roughing with a regular square corner endmill and finish with a solid carbide angle cutter. That way you get quality and quantity with minimal cost. Check out my video on youtube. If you are interested, send me a dimensioned drawing, and I will send you a program at no charge. Please include type of mill, endmill choice for roughing and material description.

[nomedia="http://www.youtube.com/watch?v=E3AqIZURMbI"]YouTube- HIGH SPEED MACHINING(REALLY HIGH!!!)[/nomedia]

[mcphill]

I would suggest 3 axis roughing with a regular square corner endmill and finish with a solid carbide angle cutter. That way you get quality and quantity with minimal cost. Check out my video on youtube. If you are interested, send me a dimensioned drawing, and I will send you a program at no charge. Please include type of mill, endmill choice for roughing and material description.

What's the "trick" there? Just super high spindle speed with correspondingly high feed rates? What material is the tool? Is the block aluminum or steel? I don't even see air cooling, is that right?

[jamesu229]

Carbide endmill, two parts, 1st 1018 steel, 2nd heat treated 17-4 stainless steel. No air, mist or any other type of cooling. The tricks
1550 sfm, conventional cut with carbide, absolutely no cooling applied, chips are not discolored, part is cool, endmill can be held without burning your hand after 5 minutes of serious cutting.

[pinguS]

jamesu229

That is quite a good video, the angle of the shape, is this done with a straight endmill 5/8" or does the endmill have a slight angle. Also what coating is on the endmill.

If I send the part in solidworks format, even though it is very simple, I'm on Solidcam 2009, can you do that program for it. My part is only aluminium, but I would like to see times on say 316 Stainless(1.4401). I generally use 12-16mm endmills, indexable, but have few carbides lying around.
For my part in question, I always just used an angle cutter, but as stated earlier, looking to see if solidcam can help improve speeds etc...

Also what depth and width of cut are you taking? and what are the limits of you machine in feed rate and spindle machine, I don't think I have a fast spindle type.

cheers in advance..

[jamesu229]

The endmill is a straight endmill with a 45 degree helix angle. To run your part out of aluminum I would use a solid carbide four flute endmill with no edge prep on the flutes and no coating, if this is not available cobalt or hss will work fine. Use flood coolant. Maximum spindle speed. Unidirectional (climb) cut starting at the bottom of the part. set maximum step at .03 constant. feed at .03 per tooth. leave .06 for finish . 12mm to 16mm will be ok. I can work with solids. email to davidurban31740@yahoo.com

Have a great day
David