Front and back

[coryatjohn]

I searched the forum for this topic but didn't come up with anything useful. I may be searching for the wrong thing...

I have a number of projects that have both a front and back that needs to be worked on. From what I can tell, PartWorks only works with one side of a job. It would be great if I could literally flip over the part in the computer and add details that need to be cut into the back as well.

What is the practical/common way of doing this?

p.s. Please pardon my numerous questions! I am getting great answers so I keep asking...

[phil_o]

You can flip over your drawing on the computer with the mirror command. Set up your drawing with the X,Y origin in the center and be sure you work is centered on the origin (CTRL A will select ALL, F9 key will center all). Now use the mirror command to flip the drawing over. It is helpful to keep the two drawings on separate layers.
There may be a video on your Partworks disk for two sided machining.
Also try searching the Vectric forum for info on two sided machining. Vectric produces Partworks, they call it VCarve.

Phil

[bleeth]

John:

The Mirror command is the tool to flip your part visually, but if you are trying to do a relief on both sides you will need to do two drawings and register your part in the same location. Regardless of whether you are using Vectric or Artcam, they are actually 2.5D programs.
If your flip-ops is for pocketing, v-carving, or some other general vector driven tooling you can create the paths but the 3-d view window won't show both the front and the back carving at the same time. True 3-d design work takes a different type of software.
The layer tools are very helpful here.
You don't need to assign 0,0 to the center of your model though-the mirror tool will flip all vectors on center of x or y axis depending on your selection.

When I do something that needs flip ops I generally draw it all from the front on one drawing and then save to another name (as in Guitar 1-back) and then flip it and toolpath here just to be safe. With the different vectors defining my tooling having different layers (like control pocket, neck pocket, etc on front and control cover on the back, I then simply turn off visibility of the vectors I don't want to use when toolpathing.

For something complicated like a 2 sided door panel with if the two sides are different I'll definately do two seperate drawings and just make sure my overall boundary vector is in the same location relative to 0,0 for registering on the table. You don't have to have two drawings-It just seems to make it less mistake prone for me.

[steve_g]

John...

There are many ways to skin the proverbial cat... however what works in one situation often won't work in another. The critical element in all of this is to keep track of where you are... By this I mean you have to know where you are in relation to previous cuts on the other side. One way to do this is to use jigs and fixtures that were precisely located with locating dowels using the CNC. Holding fixtures can become necessary when there are no reference points of the original remaining... Sometimes that fixture is a part of the original material that is still attached to the project with tabs or lugs, (My term for heavy tabs) a frame or spots of material that retain original locating information. If the face of the project retains enough original thickness, simple dowels are the easiest way to re-locate (keep in mind that dowel locations flip also when you do the flip).

A typical short run production for me would involve running a file, move all parts one fixture to the left, run the same file again, repeat. This can involve several fixtures that include flips and involving my 2nd Z axis as a defacto tool changer.


I've not done it, but an indexer can be used to hold and flip a part... even doing 4 side machining.

I hope this has given you a starting place to come up with unique and productive methods of locating your parts. It has been said that hold down methods are the most challenging part of CNC work... This takes that challenge one step beyond and adds the factor of precision locating, often not necessary in one sided cutting. Every added step also adds to the cost of failure... losing previous work.

SG

[coryatjohn]

Excellent information, especially about the precise location issue when flipping a part. I've been thinking about that for months.

I'll be experimenting with flip-side machining in the next few days. Lots of fun stuff to learn!

[adrianm]

The Cool Cubes project on the Projects page - http://shopbottools.com/mSupport/projects.htm - is a great intro to how to lay out double sided jobs.

[myxpykalix]

John here is how i would do it, see pic. draw your part to include the outside dimension of your material, the location of your dowel holes and area of your part for side A

Then keep all those things the same and place side B in the area labeled "part to be carved" so that when you flip the material the part to be carved is in the same X,Y location on your table.
Also you need to be aware of your material thickness and depth of each side that is to be carved so you don't carve too deep into the material.

[coryatjohn]

"It has been said that hold down methods are the most challenging part of CNC work..."

This reminds me a lot of concrete work. The hardest part of concrete (no pun intended) is setting the forms. Too little rigidity and the thing explodes and there's a mess. Too much and it wastes time and materials plus it makes it hard on disassembly. Just right and everything goes smoothly.

[gundog]

I do this all the time the parts I am making are a mechanical rollers that need a pocket on both sides. I draw the part with all the vectors on one layer so I know they are in the right place I add two .125" drilled holes in the scrap of the sheet one on each end at opposite corners.

I save one file as the front side and flip all the vectors vertically and save as the back side. I use the .125 holes to locate the back side I use a lazer edge finder to do this. I have also made some small dowel pins to stick in those drilled holes with a machined X in the middle of the pin (you could replace the machined pin with a small phillips head screw).

What you have to remember is the vectors must be centered in the material and when you flip you need to remember if you flip vertically on the computer you must flip the sheet vertical physically or it won't come out right. When I do this I always flip vertical I remember this because I can't flip a sheet horizontal on the table physically in the shop because the sheet would hit the ceiling.

When I have flipped the sheet I send the spindle to the coordinates I have marked and move the sheet to line up to the lazer. When the lazer lines up on both drilled holes the material is in the right position and I turn on the vacuum hold down. I have heard people that use dowel pins in the table top but I don't want dowel pins in my vacuum table for other projects. The other problem is the material I get is usually not square or the exact same size from one order to the next so this method works the best for me.

Here is the parts I do this on you can see when the sheet is flipped the parts are oriented differently because of the way the parts are nested. They always come out perfect using this method.

[dana_swift]

@John - your wondering about finding a known location when you flip a part over is easy "if" you can cut a hole through the material, perhaps in a sacrificial area.

Ideally you make two holes lined up in the X or Y axis to make squaring the part up easier.

Then use the copper sweat fitting technique I wrote about in this thread:
http://www.talkshopbot.com/forum/showthread.php?t=16539

You will be able to locate the same position on the other side with a reliable accuracy of 0.002" if your machine is setup correctly. The repeatability will be better than 0.001" if you run the center in hole routine multiple times.

Also.. be sure to run the center in hole TWICE. The first time the flutes in the bit cause a slight error, the second time that is removed and you get the correct center. This will make sense after you have done it a few times.

Hope that helps-

D

[coryatjohn]

Great tips. I appreciate them. I bought a laser edge finder. Sounds like a really useful gadget.

I see there is a good requirement for repositioning a part for rework or flip sided machining. These tips will help me accomplish that task.

Thanks!