[Philbobb]

If you use a fixture plate maybe a drop of super glue in the spots of the stock where the parts are before securing to the plate. Machine at normal loads till around 10 thou depth left, then a last cut down to proper depth or an extra 5 thou. The super glue would hold the parts in place for the last DOC, then break them free of the fixture.

[BAMCNC.COM]

Make your Z zero the bottom of the plate, NOT the top of the plate. Many people don't realize this, but this way the thickness will be exactly what you want after you face the material/part.

For example, the Z Zero on my Robodrill is the vise bed, and it will never change from that. I will never put a probe in my Robodrill again, there is no need, draw everything in CAD so it comes out EXACTLY as planned.

[MetalShavings]

I can't quite wrap my head around zeroing the Z axis on the bottom of the plate. I've been doing it just the
opposite for so long that I'm having a hard time processing this information.

In my mind I automatically think that if I do that my end mill will crash into the table or the jaws of my vice.
Can you clarify in a way that a two year old can understand? That might help me to picture exactly how this
would work.

I'll be making another batch of these next week. It would be nice if I could get my 770 mill to do all the work without having to go back and do alot of post-machining work to them.

MetalShavings

[mountaindew]

The cam strategy I would use is very similar to method outlined in bamcnc post above.
I tend to set the z zero point at top of material of first side. This allows all operations on this to be completed not knowing or caring what the actual thickness is of raw material is.
And these operations are programmed to complete the part down to a specified depth in the design or bottom of part.
Then the part is flipped and mounted on fixture. This side of part the z zero point will be set to bottom of part. "This is the finished surface of the previous side"
A surface operation setup in cam at this point can mill off excess material down to exact thickness because it is using the difference between thickness designed and the z zero point set at bottom of part.
Using this method allows the surface operation to run never knowing where the top of the raw material is because it could vary but it does know where the top of part is exactly.
About the only concern to the user or cam program has for the final surface operations is how big a depth of cut is this going to be averaged and to setup feeds and speeds that can cover any or all the variances.
in theory using this method you could make parts from material that varied in thickness by say 1/4" or more and always end up with correct part dimensions.

Something to consider

Edit:
After reading the next couple of posts I can also add if you use a nominal material that does not vary much a user can also avoid setting the first z zero point at top of material if it will always be close to the same. Your cam program can then first Safely do a surface op and all other ops for that side based on a offset from bottom. Then part is flipped and again all ops are completed from z zero set a bottom and all ops are calculated from bottom to top or designed thickness of part.

The example I detailed first is handy to safely make parts from raw material that can vary a great deal and helps the user make parts from rougher sized material and not need to re cam the part based on a new raw stock size.

[SCzEngrgGroup]

Zeroing to the bottom of the workpiece, or top of the fixture, can save a LOT of hassles.

First, the coordinate origin generally doesn't move as you machine the part. Whereas, if you zero to the top of the workpiece, once you machine away the top surface, you've lost your reference.

Second, as pointed out, zeroing to the bottom lets' you machine the piece to exact height, whereas zeroing to the top requires first measuring the thickness of each piece before machining if you want exact height.

Third, It let's you know at a glance, how much "safe" clearance you have between the end of the tool, and the top of the fixture, vise, etc. If the Z height in the G-code is >0, you know you're clear. You also know any Z height greater than the max. material thickness will not make contact with the workpiece.

Many, if not most, of the parts I make would require several fixtures to machine zeroing off the top, whereas zeroing off the bottom, I can generally do it all in a single fixture, even if the part needs to be re-positioned (flipped, rotated, etc.) several times during the machining process.

Where you set your zero is, largely, immaterial, as it simply shifts your Z coordinates up or down. If you're working with 1/2" stock, zeroing on the top of the part, your cuts will all be between Z=0 and Z=-0.5. If you're working with 1/2" stock, zeroing on the bottom of the part, your cuts will all be between Z=+0.5 and Z=0. Nothing else changes. But, as described above, zerolng on the bottom of the part can save a lot of hassles and time.

Regards,
Ray L.

[AUSTINMACHINING]

I can't quite wrap my head around zeroing the Z axis on the bottom of the plate. I've been doing it just the
opposite for so long that I'm having a hard time processing this information.

In my mind I automatically think that if I do that my end mill will crash into the table or the jaws of my vice.
Can you clarify in a way that a two year old can understand? That might help me to picture exactly how this
would work.

I'll be making another batch of these next week. It would be nice if I could get my 770 mill to do all the work without having to go back and do alot of post-machining work to them.

MetalShavings

What he is saying, and the way I do it... Say your stock is sitting on parallels in the vise. So lets say you have parallels that are .1" below the top of the vise jaw. The bottom of your stock is resting on the parallel. Touch off zero on the top of the parallel (which is the bottom of your stock) as your reference point. In you CAM, you origin has to be in the same point. You also have to insure you have enough excess stock height so that you lowest cut is > .1" above the parallel (Top of vise jaw) so you don't hit the vise jaw. When you flip the part, the origin is already set for the next operation and you part will be exactly the thickness as designed. If you model everything in cam and simulate, you will see exactly what is going to happen.

[MetalShavings]

What he is saying, and the way I do it... Say your stock is sitting on parallels in the vise. So lets say you have parallels that are .1" below the top of the vise jaw. The bottom of your stock is resting on the parallel. Touch off zero on the top of the parallel (which is the bottom of your stock) as your reference point. In you CAM, you origin has to be in the same point. You also have to insure you have enough excess stock height so that you lowest cut is > .1" above the parallel (Top of vise jaw) so you don't hit the vise jaw. When you flip the part, the origin is already set for the next operation and you part will be exactly the thickness as designed. If you model everything in cam and simulate, you will see exactly what is going to happen.

OK; I got you now.

I have to ask though; isn't this basically what we're doing when we reference the Z-axis on the top of the stock, then
flip the stock around so that it sits at the same height it was in with the first stage of our milling?

Wether it is or it isn't doesn't really matter at this point. It still sounds like it may be worth a try. Thanks.

MetalShavings

[daniellyall]

grab a piece of stock put a mark on at the bottom left corner flip it over where the mark is, is where your xyz ref point is for the second op. you can do the same in your cam. yes you can do the top but when you flip it over it`s not in a safe plane.

if you ref the bottom left front corner first, for the first op you set the cut depth to the top of the vice jaws, you just have it so it has 1/3 not cut (1/3 in the vice) then when you flip it you have 1/3 to cut 1/3 above vice jaws, so if you need to take any material off to get to the correct thickness you wont hit the vices jaws. for the second op it`s top left back 180 roll over

if what you are cutting out is 15 mm high and you use 20 mm stock, you set it so there is 15 mm above the jaws 5 mm below when you flip it use a set of soft jaws with the pattern cut in to them at a depth of say 5mm that will hold all the parts in places then all you need to do is plane the top off and do any cutting needing to be done on the other side and there is 15 mm to play with, 5 mm to cut of and 10 mm above the soft jaws.

it just makes it so there is less chances of hitting the vices you just need to make sure your first op is bang on

[AUSTINMACHINING]

OK; I got you now.

I have to ask though; isn't this basically what we're doing when we reference the Z-axis on the top of the stock, then
flip the stock around so that it sits at the same height it was in with the first stage of our milling?

Wether it is or it isn't doesn't really matter at this point. It still sounds like it may be worth a try. Thanks.

MetalShavings

No,
When you flip the part it won't be at the same height because you already machined some off in the fist operation.

[BAMCNC.COM]

It's very simple, the best approach is to not think about, or worry about it. Your cam will take care of it.

Zero on the top of softjaws, now draw and mill them to be step jaws (zero at the same spot on mill, and cad). Ok, now make your zero the top of the step on your machine and in the program. Ok, now this zero NEVER moves... EVER. Put the raw stock in, who cares how tall it is, just go to work milling while your zero is on the bottom of it. I don't really have time to explain, but it is the the ONLY way way to do this accurately.

I'll make a youtube video of it this weekend. Keep an eye on my channel

[MetalShavings]

I must have some kind of dyslexia thing going on because just as some of your replies start to make sense to me, they start to loose that sensibility when I think back to my original posts.

I'm going down today to buy the metal stock to make up a set of "Soft-Jaws" for this specific project. It's hard to tell from the pics I posted but these parts are really small. They're about 1/2"x1/4"x5/8" overall; although the geometry is a little more complex than just a simple rectangle. I mention this because I've had to order some 3/32" end mills to use for slotting the smallest profile sections of these shapes.

I did take the time to view "tacticalKeychains" video listed above by BAMCNC. I'll just have to wait and see if it's going to work for me. I'm really hoping it does work because within the last couple of days I've had a few more request to purchase one of these tiny parts.

MetalShavings

[kstrauss]

Don't waste your time making soft jaws but buy them from Monster Jaws. Their prices are about the same as I would have to pay for the raw stock and they arrive ready to use.

[Steve Seebold]

Material for soft jaws will cost you about $9.00.

Monster Jaws sells them machined on all 6 sides for about $11.50. That means you have to machine them for $2.50. You might be fast, but I'll guarantee you ain't that fast.

[CadRhino]

I want to see the video Brad. I have my coffee in hand so get it loaded

One thing you can do if you don't want change all of your current CAM programs, you can set your zero off of the vise/jaws/table as folks are suggesting and then move your indicator up to the proper height and re-zero your machine for that height (as opposed to physically measuring off of your stock).

The best method I am finding out is to zero from the bottom of the fixture like folks are recommending but this is one work-around for parts I CAM'd with the zero on top of the part.

It's very simple, the best approach is to not think about, or worry about it. Your cam will take care of it.

Zero on the top of softjaws, now draw and mill them to be step jaws (zero at the same spot on mill, and cad). Ok, now make your zero the top of the step on your machine and in the program. Ok, now this zero NEVER moves... EVER. Put the raw stock in, who cares how tall it is, just go to work milling while your zero is on the bottom of it. I don't really have time to explain, but it is the the ONLY way way to do this accurately.

I'll make a youtube video of it this weekend. Keep an eye on my channel

[snovak240]

Get in touch. I have been making about 6 different triggers along with some stuff thats the size of an eraser if you removed it from the metal it is attached to the pencil. Maybe I can help.

[MetalShavings]

Don't waste your time making soft jaws but buy them from Monster Jaws. Their prices are about the same as I would have to pay for the raw stock and they arrive ready to use.

If I can make these myself, it's not a waste of my time. One of the many reasons I bought my Tormach was to become as self-sufficient as possible.

I did look at buying pre-made soft-jaws and as you have stated, they are not that expensive but, to me neither is making my own. If it doesn't work out I can always buy them later on.

MetalShavings

[mountaindew]

Material for soft jaws will cost you about $9.00.

Monster Jaws sells them machined on all 6 sides for about $11.50. That means you have to machine them for $2.50. You might be fast, but I'll guarantee you ain't that fast.

Agree lol
Only way I found to make them cheaper and they come with the added benefit of storing in a smaller space
Attachment 291024


And the added option of making custom sizes and shapes for different needs

[daniellyall]

MetalShavings can you define your fixture in cam what cam are you using, if you can Look how TKK does it, his way is a do once correct and that`s it, you only have to define the fixture once`s as you set it up in cad

[MetalShavings]

MetalShavings can you define your fixture in cam what cam are you using, if you can Look how TKK does it, his way is a do once correct and that`s it, you only have to define the fixture once`s as you set it up in cad

I am a self-taught hobbyist. Alot of the terminology used by machinist is foreign to me. I'm not really sure what "Defining Your Fixture" refers to. I don't have any problem securing my metal stock in order to machine these little parts I'm making. My problem has been in keeping those little parts from breaking loose from the metal stock and becoming damaged in the process; not to mention the damage to my end mills.

I'm nearly done with my soft-jaws. Making them is not difficult. I am having some trouble drawing them up in my CAD software. (not the blocks per se) Using SolidWorks, I cut and pasted the original geometry that I'd previously drawn up. When I pasted it onto my new palate it ended up in the upper right corner of the SolidWorks window at an angle that did not align with the Axis of the palate. I didn't think anything of it at the time. I just kept drawing until I was finished.

Now I'm trying to figure out if or how my drawing can be aligned -after the fact- to the correct X,Y,Z Axis'. I can straighten it out in my SprutCAM software but, it's a whole lot easier when it's aligned correctly from the git-go. I'd never cut and pasted anything in SolidWorks before. This could turn out to be one of those hard lessons we "Self-Taught" people just have to go through during out learning process.

When you're self-taught, you have a situation where the teacher is just as ignorant as the student. It' a trial and error thing; mostly error.

I guess I'll mozzy on over to the SolidWorks section of this forum and see if there's a way to fix this. I'd hate to have to redraw the whole darn thing but, If that's what it takes; that's what it takes.

MetalShavings

[kstrauss]

I'm not a Solidworks guru and I'm also a self-taught hobbyist so take my suggestions with appropriate respect!

When I'm making a part that will be held using soft jaws I add a circular recess (usually 0.3 inch diameter since I mostly use 1/4 inch and smaller cutters) to the part drawing at a point outside of but near the periphery of my part. Depending on the size of my part I may duplicate the part to permit making several in one setup. I don't actually include the jaws to my drawing. In my CAM I generate a toolpath that will create a recess whose outline matches the part to be held and, obviously, a path to produce the locating recess. I often lie about the size of my cutter and say that it is 0.001 inch or so smaller than its actual size so that the holding recess has a little clearance.

I close the jaws on a spacer of scrap aluminum 0.05 thick, zero things so the aluminum spacer is roughly at the centre line of the part to be held and mill the holding and locating recesses.

Sof tjaws are great for machining the back side of a complicated part that must be machined all over.

I hope that my description makes sense. If not I'll try to locate some soft jaw samples that may make things clearer.