4th axis COR

[Mic6]

Hey all, in the Front view pic below, the center line of the indexer goes thru the middle of my 1.0 thick fixture plate mounted between centers, with that my part which is withinthe bounding box was moved up in Z .50.  Is this the correct positioning method for Center of Rotation?

 

COR Sample.mcx-9

[djstedman]

Assuming the relationship of the part is correct relative to the centerline of the rotary it should be good - ie assuming it matches the way it is positioned in the machine.. then all your coordinates should work

[Mic6]

Yes, X and Y are locating on pins relative to center line.  I started milling C'bores and as you can see in the pic, the helix starts above the surface, but IRL, as the angle increases (to the right) the tool hits the part before it begins the helix bore.  I checked COR height in the machine, the height is exactly what it is in Mastercam.  X and Y are on pins so they can't go anywhere.  In Mastercam Y is on center line.  Verify and Backplot look perfect.  Am I overlooking something?

 

The double lines are holes slightly shifted from each other on each side of a window.

 

I measured from the table up to COR and from there up to the top of stock and it matches MC within .0006.

 

[crazy^millman]

Is doglegging going on with those rapid moves? Have you tired to G1 between the holes?

[Mic6]

Nope, no dog leg, just a nice hole to hole around a window.  The picture above is a RIGHT side view.  In this point the helix is starting above the stock.  Top of stock is where the c'bore starts, but in the machine, it's already touching the work

 

[djstedman]

When is it hitting? Is it when it goes to do the helix? or when it goes to move in rapid?

 

What is your clearance height set to?

 

From the backplot it looks like its not that high.. since its all using one zero (I assume) then your clearance height will need to be high enough to clear the 'highest' portion when it is rotated up to position.

 

Mastercam has issues with backplot and verify sometimes with showing clearance moves as they would actually happen in the machine.

[Mic6]

When is it hitting? Is it when it goes to do the helix? or when it goes to move in rapid?

 

What is your clearance height set to?

 

From the backplot it looks like its not that high.. since its all using one zero (I assume) then your clearance height will need to be high enough to clear the 'highest' portion when it is rotated up to position.

 

Mastercam has issues with backplot and verify sometimes with showing clearance moves as they would actually happen in the machine.

 

 

When it goes down to do the helix.  Clearance is set at 2.0  Yea, it's not that high, I just though MC was perfect and it would work just like backplot.  I bumped the retract and feedplanes up and I'll see how that works.

[Mic6]

Well, my counter bores have the correct depth, but now when I go to spot the thru hole, what appeared great in MC, only the hole at 0° has a visible spot. 

 

Now when I do my Hole Axis points/lines for this, the point should be at the hole centerpoint at the bottom of the C'bore, with the axis line going up to the surface correct?  I'm using Multiaxis drill.

[djstedman]

If you are working from the model, then you should be able to make your depth, top of stock and retract amounts be in incremental, then make your clearance something high enough to clear everything.

 

The only thing backplot doesn't really show correctly is how your spindle moves in relationship to the part. The reason is because Mastercam backplot shows the spindle as if it was able to move in any direction, but in your machine the spindle is locked in the vertical position.

 

If you watch backplot in side view you will see the spindle rotates around the part while the part remains stationary.. in the machine that's not how it works, but if you want it to look exact you need to cough up the dough for something like vericut where they come in and build a simulation that's exact based on your machine's kinematics.

[djstedman]

I haven't used multiaxis drill so I cant really help with that too much.. But it seems like what you said makes sense.. I would think you will want your depths and such in incremental though if you don't have them that way already.

[Mic6]

Thanks DJ, I do appreciate the feedback.  Yup everything is incremental, when I show the toolpath it looks perfect, I just can't make it match in the machine.  The heat is on and I have to get this right.

[Rstewart]

I would get away from that Multiax Drill and just do it old skewl with Planes to get the job out the door....

[crazy^millman]

I would get away from that Multiax Drill and just do it old skewl with Planes to get the job out the door....

 

Agreed. 5 Axis Drill is a good toolpaths, but seen it cause some wired issues.

 

Hate having to old school say 500 holes like we may to on a current project, but sometimes you have to go with what works.

[Mic6]

Okay Guys, I switched over to Planes by Normal for each hole.    WCS set at TOP  T/C set at each specific hole plane.

 

 

but I get this error at the angled holes.

[mkd]

is that a 5C indexer?

is your fixture slipping about A axis?

[mkd]

copy your top plane and then rotate to specified hole angle?

[Mic6]

is that a 5C indexer?

is your fixture slipping about A axis?

 

Yes, HA5C, no collet, chuck is threaded on and torqued and I put a jack underneath at each hole operation.  I put a scribe mark to watch for slippage.

[Mic6]

My brain is killing me.  I'll see you guys in the morning.  Thanks for all the help. 

[Rstewart]

I have some time to look at your file if you want...

[Mic6]

Rstewart.  Thanks, I'm looking at a file you helped me with before with angled holes.  It was 4 holes and each plane is at the center of rotation, but as I click on each plane in the Plane manager, I can see the Gnomon changing angles.  I used, Plane by Normal and clicked the Axis line, but the Gnomon stayed at the axis line.  How do I get the Gnomon to the COR?

[djstedman]

OK  a couple things.

 

That Error usually comes up when you don't actually have a fourth axis, because it wants to rotate your rotary table, but you don't have one configured in your machine def. or alternatively it can come up if the plane it is trying to rotate to is impossible using the current machine definition. So first question is, do you have a fourth axis machine setup that has a rotary table configuration with the rotary setup on the X axis of the machine?

 

Assuming you do have the machine def. correct, are the holes only rotated in one direction? If the normal for those planes are tipped in two directions - around X and around Y then Mastercam will give out that error because it cannot rotate that way. So you would need a 5 axis or special fixturing to align the part.

 

 

Then on to the planes..

 

First, if you're using one work offset based on centerline, you should have no offsets for your origins in your new planes, all three numbers for offset(in view coordinates) should be set to zero.

 

Second thing, if you want it to use one work offset for all the paths, you then need to assign a work offset by checking the work offset checkbox and then setting the value to 0-5 (for G54 to G59)

 

When you go to set the work offset you will probably get a pretty annoying dialog box whining if you should reset all for this view etc.. to keep things simple you would probably want to choose the option something like update work offset for this toolpath without changing the view / plane or something along those lines.. this way it doesn't screw any other paths up behind the scenes unintentionally.

 

If your having any issue creating planes it should be relatively easy..

 

Creating the planes should be easy assuming they are only angled around X..

 

As someone else said just rotate your top plane..

 

First look at part from the side.. and on a new level create some lines along the axis of the holes.. those should allow you to measure the rotational angle off of zero..

 

Then look at part in top view and rotate around X to get that angle - then name and save current view - I suggest naming them something that is easily identifiable later.

 

If you do it that way that view should then correspond to one hole.. then just do that for all the holes ..

 

Anyhow .. hope any of this helps.. as rstewart said.. if you could post the file it would be a lo9t easier to diagnose..

[CJep]

Mic are you using the center of rotation as your Y/Z zero?

When you created your custom planes did you maintain the pos X direction?

[Mic6]

DJ :  Thanks man, much appreciated.  I'll check out all the stuff you mentioned.

 

CJ :  Yes, my WCS is on center of rotation.  When I created planes I did "by Normal" and used the hole axis lines.

 

 

 

 

****SAMPLE FILE IN ORIGINAL POST****

[CJep]

If you're going to use custom planes for rotation the origin for those planes should be the same as the center of rotation.

Rather than using plane normal, I create vectors from the hole geom then use planes dynamic to align the axis.

[Mic6]

Okay so all my Planes are now set at COR, I can see the toolpaths going in at angles, but I'm still getting the error about machine achievable X axis.  The holes are only going in one direction.