Ok so at work sometime we will run into a part that needs a fixture to be made to run it correctly so I question is about programming using a daytum hole as x y zero how do you go about that in my head I’m thinking I make the hole like x distance off the left side and back side and just figure out from that location where the part will sit and then what the x and y location will be so let’s say for example the part is 2 inches from the daytum center then and I want the hole 3 inches from that left X so I would make my X for that hole X5. Correct?am I thinking correctly?
1 Like
That seems to be correct. I generally build the fixture on a piece of paper first. Then transfer to the machine.
That’s pretty much what I was picturing in my head when thinking about it
1 Like
just make sure you engrave or stamp the fixture with the coordinate of your hole so you know for next time
1 Like
If the print calls for the datum to be a hole, then my hole is what I program zero to. If you want to shift the X-Y position from a corner of material, do so, but thereafter pickup the hole to be your X-Y position. My practice if the print called for a datum not on a corner would be to use a G56, G57, G58, for the datum position. I save G54 to be the upper left hand corner of material, where Y is the hard vise jaw and X is the hard stop established either by end of jaw, or a mill stop below top of vise jaws.
1 Like
Hi,
I use mastercam, and this is how.
Create a fixture plate, if in vise, 0/0 is upper right corner. Place this model on a higher level
say 100.
Create a new mcx dwg of the part/parts, default level is #1.
Open the fixture dwg and use “file merge” to import the mcx dwg of the part/parts.
Select the part and use “translate/transform” to locate the part where you want it on the fixture.
You will now copy the datum hole location to level #100. Turn off level #1, you now see the
fixture plate with the datum hole. Drill/ream or use a shoulder bolt to locate the part. The part and fixture plate become one and the same. Use 1 work offset for the fixture. Save this dwg
with another name and use it to contour the part.
I don’t know if this is possible in fusion 360.
Regards
Magicman
1 Like
Exactly right but this is why I hate MasterCam and love Inventor all I have to do it change 2 Numbers. Then I can setup as many offsets as I want. Yet MasterCam is still a powerful CAD for wire for now lol.
1 Like
You can place as many parts as you want on 1 fixture,
and you only need 1 work offset for the machining
operations.
1 Like
yes you can do it that way. I do it with individual offsets so i have more control over tooling. That is depending on what type of fixture I will be running. If it has 10-20 parts I will go 1 offset, and if its fast running parts being roughed out or have open tolerances. Multiple ways to skin a cat as the saying goes.
1 Like
If your fixture is not precise or has moving parts, you could always use G10 for each individual work location.
1 Like
Courtesy of hpdg in Practical Machinist forum -
G10 is just a method of entering offset values from the program.
G10 L12 G90 P1 R0.5 enters the value of 0.5" into the tool diameter table for Tool 1.
G10 L2 G90 P1 X-5. Y-5. Z-5. enters those XYZ values into the work offset table for G54.
It is also possible to increment the values by using G91 in the command. On a Haas which can call a subroutine with an L count you can move the work offset for each call.
G10 L2 G91 P1 X-2. M97 P1000 L5 will increment G54 a-2. along the X axis and call subroutine N1000 five times. Personally I do not like this because I have the feeling I might get lost.
G52 creates a subsidiary (‘daughter’ in some manuals) work zero with reference to the active work zero.
G54
G52 X-2. creates a work zero X-2. from the G54 location.
G10 L2 and G10 can be used almost interchangeably and I think it is mostly personal preference.
I find G52 is particularly useful for tool length offsets when working with rotating fixtures. The tool lengths can be set to a fixed reference point then G52 used to shift the tool offset down to the highest point on the part at each orientation of the fixture.
G52 is similar to G92 the difference is that with G52 you specify the location with reference to an known location; you know where you are.
With G92 where you are when you command G92 becomes the work offset location and all other moves are done with reference to this. Now if you command G92 several times in different locations you can get a bit lost about where you are in machine coordinates. It can be sorted out if your machine can use G53 because this uses the machine coordinate system so G53 X-2. Y-2. just moves to X-2. Y-2. and then a G92 makes that the current work offset.
They can all be used with other axes such as A or B and G92 can be useful with a rotary when doing something that needs a lot of rotations; you can reset the A work offset back to ‘zero’ with G92 without having to ‘unwind’ the rotary back to machine zero.
3 Likes
Thats a good write up on G10
1 Like
so if i am understanding correctly will the g10 L2 x-2. move the x0 down two inch?
i guess my question is there is a part that we run at my place of business that gets an engraving on the side and the way they choose to run them is one vise at a time with a g54,g55,g56,g57,g58 deal well the way i run them is stacked all in one vise from back to front and i can run like 20 at least at a time in this manner but the way i accomplish this is i add .25 of an inch to each offset and basically make the part behind it the hard jaw and Y zero so i end up with like g54 being y-10. and g55 being y-10.25 g56 is -10.5 g57 -10.75 and g58 becomes -11. so my question is could i use g10 in this manner to say shift the Y forward on each change and time it does the sub program by like .25 so for instance if i wanted to do 5 at a time could i do
g00 g90 g54 x1. y-.125 s7500 m3
g43 h z
g1 z f
p98 p2
g10 L4 g91 y-.25 m98 p2
and it do what I’m doing but faster?