Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Fixturing and Center of Rotation Questions


Greg_J
 Share

Recommended Posts

Hello,

I have a 4 axis HMC that we manufacture a part family on and over the years the parts have become more complex.

We make the part in 3 setups.

First setup is on magnets on a tombstone and we use G54 B0. and we machine whiteness marks for part pickup on setup 2.

Second setup we mount fixture plates to the finished faces from setup 1 that use a Schunk clamping system mounted to 4 legs that we and lay the part down so we can machine features at B0, B26, B90, B180 and B270 each angle having its own work offset G55-G59,

Third setup, we take off the pull stud used by the Schunk and set the part back up on the magnets and complete the 3rd setup. Unfortunately the fixture holes get milled away on this setup so to aid in work holding we use a bar clamp over the part. This setup uses G54 and B0.

I want to change the second setup. 

I want to machine the part on the center of rotation so I can machine on any angle with one work offset instead of the angles and offsets listed above, I can use shorter tools and reach into areas that are harder to reach.

I would make a plate that would accurately mount to the machine table and that would have pockets that would match the size and shape of the fixture legs. I would engrave the part number in the pockets for easy identification for the operators and engrave the orientation. The center of the part would be center of rotation (X and Z origin) and they would only have to set the Y axis origin for each part and make sure the part was in the correct orientation to B0.

It all sounds good to me because we do it on our VMC that have a rotary axis less the fixture plate we just use a chuck, but is there anything that I am missing?

What sort of issues happen with setup like this? I may be overly optimistic about this change? Accuracy matters so if the parts are too accurate they parts are tough to fit together, which would take more time to setup.

Any help, ideas or criticisms would be appreciated.

See reference image below.

image.png.30f476e32619f09afc91ab88db608528.png

Greg

Link to comment
Share on other sites

Nothing I can think of seeing your picture and explanation. Issue is how much movement can be expected and how will that effect the overall quality of the part? Different fixture offsets allow each bore to be dialed in, but is that needed? Without knowing tolerance and GDT requirements hard to say. Shorter tools and a more rigid setup are hard to beat so having those in your favor shouldn't hurt is my thinking. HMC's are normally stronger than a VMC so you do have that going to you also.

  • Like 1
Link to comment
Share on other sites

Thanks Ron.

We have pretty open tolerances. The biggest concern is the bores which we bore half and half and we would adjust the X value of the work offset after each cut to keep the concentricity with in tolerance and minimize miss match. Not sure how that will work out using fixture plates, we don't take one finish cut we take several and adjust them after each pass.

 

 

Link to comment
Share on other sites
1 hour ago, Greg_J said:

Thanks Ron.

We have pretty open tolerances. The biggest concern is the bores which we bore half and half and we would adjust the X value of the work offset after each cut to keep the concentricity with in tolerance and minimize miss match. Not sure how that will work out using fixture plates, we don't take one finish cut we take several and adjust them after each pass.

 

 

Would a Twin Bore with extender that allowed you to machine through one side and hit both through areas work? I see the step diameter on the end, but I have done that where I have Twin Bored a through hole then use it to align the other side and now alignment issues are solved from one side to the other.

Link to comment
Share on other sites
On 2/9/2021 at 1:44 PM, Greg_J said:

Hello,

I have a 4 axis HMC that we manufacture a part family on and over the years the parts have become more complex.

We make the part in 3 setups.

First setup is on magnets on a tombstone and we use G54 B0. and we machine whiteness marks for part pickup on setup 2.

Second setup we mount fixture plates to the finished faces from setup 1 that use a Schunk clamping system mounted to 4 legs that we and lay the part down so we can machine features at B0, B26, B90, B180 and B270 each angle having its own work offset G55-G59,

Third setup, we take off the pull stud used by the Schunk and set the part back up on the magnets and complete the 3rd setup. Unfortunately the fixture holes get milled away on this setup so to aid in work holding we use a bar clamp over the part. This setup uses G54 and B0.

I want to change the second setup. 

I want to machine the part on the center of rotation so I can machine on any angle with one work offset instead of the angles and offsets listed above, I can use shorter tools and reach into areas that are harder to reach.

I would make a plate that would accurately mount to the machine table and that would have pockets that would match the size and shape of the fixture legs. I would engrave the part number in the pockets for easy identification for the operators and engrave the orientation. The center of the part would be center of rotation (X and Z origin) and they would only have to set the Y axis origin for each part and make sure the part was in the correct orientation to B0.

It all sounds good to me because we do it on our VMC that have a rotary axis less the fixture plate we just use a chuck, but is there anything that I am missing?

What sort of issues happen with setup like this? I may be overly optimistic about this change? Accuracy matters so if the parts are too accurate they parts are tough to fit together, which would take more time to setup.

Any help, ideas or criticisms would be appreciated.

See reference image below.

image.png.30f476e32619f09afc91ab88db608528.png

Greg

I'm sorry, I don't have any input on your process, but I'd like to know more about the magnet workholding!!!

 

What type of magnets are you using that hold well enough for machining??

Link to comment
Share on other sites
4 minutes ago, JB7280 said:
On 2/9/2021 at 1:44 PM, Greg_J said:

Hello,

I have a 4 axis HMC that we manufacture a part family on and over the years the parts have become more complex.

We make the part in 3 setups.

First setup is on magnets on a tombstone and we use G54 B0. and we machine whiteness marks for part pickup on setup 2.

Second setup we mount fixture plates to the finished faces from setup 1 that use a Schunk clamping system mounted to 4 legs that we and lay the part down so we can machine features at B0, B26, B90, B180 and B270 each angle having its own work offset G55-G59,

Third setup, we take off the pull stud used by the Schunk and set the part back up on the magnets and complete the 3rd setup. Unfortunately the fixture holes get milled away on this setup so to aid in work holding we use a bar clamp over the part. This setup uses G54 and B0.

I want to change the second setup. 

I want to machine the part on the center of rotation so I can machine on any angle with one work offset instead of the angles and offsets listed above, I can use shorter tools and reach into areas that are harder to reach.

I would make a plate that would accurately mount to the machine table and that would have pockets that would match the size and shape of the fixture legs. I would engrave the part number in the pockets for easy identification for the operators and engrave the orientation. The center of the part would be center of rotation (X and Z origin) and they would only have to set the Y axis origin for each part and make sure the part was in the correct orientation to B0.

It all sounds good to me because we do it on our VMC that have a rotary axis less the fixture plate we just use a chuck, but is there anything that I am missing?

What sort of issues happen with setup like this? I may be overly optimistic about this change? Accuracy matters so if the parts are too accurate they parts are tough to fit together, which would take more time to setup.

Any help, ideas or criticisms would be appreciated.

See reference image below.

image.png.30f476e32619f09afc91ab88db608528.png

Greg

I'm sorry, I don't have any input on your process, but I'd like to know more about the magnet workholding!!!

 

What type of magnets are you using that hold well enough for machining??

Electro magnets would be used for workholding, commercial magnetic vises and chucks are available from different manufacturers...

Remember if you are working with magnets keep the cnc door closed...

Link to comment
Share on other sites

 

 

We use Earth-Chain ECB-210 permanent magnet, each magnet has the ability to hold up to 2100kgf with the correct surface finish.

https://www.earth-chain.com/ecb.html?cid=29

 

In my setup we use 4 magnets horizontally mounted to a tomb stone with 2x4x6 block under the forging.

Our forging sizes range from 2500 lbs. to 12000 lbs. I've been using them for 12+ years now and we have never had the part move while machining.

We run a 3" high feed cutter taking .08 doc up to 600 ipm and a 4" face mill taking .25 doc at 60 ipm on these parts with no issues.

  • Thanks 1
Link to comment
Share on other sites
34 minutes ago, Greg_J said:

 

 

We use Earth-Chain ECB-210 permanent magnet, each magnet has the ability to hold up to 2100kgf with the correct surface finish.

https://www.earth-chain.com/ecb.html?cid=29

 

In my setup we use 4 magnets horizontally mounted to a tomb stone with 2x4x6 block under the forging.

Our forging sizes range from 2500 lbs. to 12000 lbs. I've been using them for 12+ years now and we have never had the part move while machining.

We run a 3" high feed cutter taking .08 doc up to 600 ipm and a 4" face mill taking .25 doc at 60 ipm on these parts with no issues.

That is super helpful information, thanks for sharing!

Link to comment
Share on other sites
On 2/9/2021 at 1:44 PM, Greg_J said:

Hello,

I have a 4 axis HMC that we manufacture a part family on and over the years the parts have become more complex.

We make the part in 3 setups.

First setup is on magnets on a tombstone and we use G54 B0. and we machine whiteness marks for part pickup on setup 2.

Second setup we mount fixture plates to the finished faces from setup 1 that use a Schunk clamping system mounted to 4 legs that we and lay the part down so we can machine features at B0, B26, B90, B180 and B270 each angle having its own work offset G55-G59,

Third setup, we take off the pull stud used by the Schunk and set the part back up on the magnets and complete the 3rd setup. Unfortunately the fixture holes get milled away on this setup so to aid in work holding we use a bar clamp over the part. This setup uses G54 and B0.

I want to change the second setup. 

I want to machine the part on the center of rotation so I can machine on any angle with one work offset instead of the angles and offsets listed above, I can use shorter tools and reach into areas that are harder to reach.

I would make a plate that would accurately mount to the machine table and that would have pockets that would match the size and shape of the fixture legs. I would engrave the part number in the pockets for easy identification for the operators and engrave the orientation. The center of the part would be center of rotation (X and Z origin) and they would only have to set the Y axis origin for each part and make sure the part was in the correct orientation to B0.

It all sounds good to me because we do it on our VMC that have a rotary axis less the fixture plate we just use a chuck, but is there anything that I am missing?

What sort of issues happen with setup like this? I may be overly optimistic about this change? Accuracy matters so if the parts are too accurate they parts are tough to fit together, which would take more time to setup.

Any help, ideas or criticisms would be appreciated.

See reference image below.

image.png.30f476e32619f09afc91ab88db608528.png

Greg

I love the setup. 

I would recommend adding a hole in the center of the plate, where the COR would be, and mount a 1" Gauge Ball for calibration, if your shop uses Probing. That way you have a reference at any angle, which can be referenced if you need to shift the work offset.

I really like Ron's idea of a twin-bore with extended holder, that could reach through. Even if it wasn't the true "finish bore size", it would give you a reference that you could probe after rotating the pallet 180 degrees.

For Roughing through those bores, you could do it half/half with an extended tool. I personal love Capto C8 extensions for this sort of thing. You can hang a tool out 12" from the gauge line, and have it still be fairly rigid. This is especially true if you use High-Feed Mills, since the nature of the tool tends to put the force into the spindle axis, rather than acting as strictly a "bending moment".

Programming from COR on a horizontal has a ton of benefits, but you'll still need to build in the ability to correct for errors into your process.

Are you going to use G52 Work Shift for setting COR? I like that method, as it still allows you to use "local work offsets" if needed, and your Probing/Error Corrections would still get applied to G54, G55, Etc, but the amount of correction is easy to read. G54 = X-0.0021 Y0.0004 Z-0.0005, is easy for the Operator to judge how far off the correction is, for a particular Work Offset. (That way you just probe a feature, and just use the XY or Z error values to adjust the Work Offsets (which are already 0, 0, 0). (Only G52 has the COR values.)

Be aware that you'll need to check the calibration of the COR Values, to make sure the offset hasn't drifted with temperature.

  • Like 2
Link to comment
Share on other sites

Do you have a link to a twin bore?

We currently use Sandvik Divibe bars, not cheap.

Those parts we make have single, double, triple and quad bores through ranging in size from 3.500 to 8,000 with a +/- .001 and 32 surface finish.

We made a triple out of solid incoloy 925 last month, 330 hours machine time, fortunately it was one of our smaller size parts.

Unfortunately we do not have probing on our Toyoda 1250 machine we use dial probe and it would be very touch reaching to center of the table, I was thinking of putting tooling ball locations on the 4 corners and referencing them when needed.

I really do like the G52 suggestion and making minor adjustments on G54.

  • Like 1
Link to comment
Share on other sites
1 hour ago, Greg_J said:

Do you have a link to a twin bore?

We currently use Sandvik Divibe bars, not cheap.

Those parts we make have single, double, triple and quad bores through ranging in size from 3.500 to 8,000 with a +/- .001 and 32 surface finish.

We made a triple out of solid incoloy 925 last month, 330 hours machine time, fortunately it was one of our smaller size parts.

Unfortunately we do not have probing on our Toyoda 1250 machine we use dial probe and it would be very touch reaching to center of the table, I was thinking of putting tooling ball locations on the 4 corners and referencing them when needed.

I really do like the G52 suggestion and making minor adjustments on G54.

I suppose if you had the Fixture Plate made accurately enough, any reference would do. It is simple enough to probe one of the Ball tops at B0. and the others at B90, B180, and B270, to check and see if your fixture plate is truly aligned to center.

Do you have the option of machining Ball Lock Receivers into the Machine's Table? That would eliminate a lot of setup headaches that could occur, by making the fixture plate repeat to within about 0.0002-0.0004.

Bob's suggestion of Dynamic Fixture Offset (G54.2) is also a good one. But it would still require you to have some method of accurately calculating and setting the Center of Rotation parameters. This is easier said, than done, without a Probe installed.

My suggestion on using those 4 tooling balls would still be "have someone machine an accurate center hole", and also put the Tooling Balls at each corner with as tight a true position tolerance as you can get.

If you go with a Tooling Ball on each of the corners, you could actually measure both the left and right ball when checking each 90 degree face. That would make it easier to adjust the G52 XYZB Positions, as you could potentially just adjust the B-Axis offset on G52, to get the face perfectly perpendicular.

38 minutes ago, crazy^millman said:

Many make them now a days no preference and all the majors have their own stuff also.  

BigKaiser: Link

These are also good, but my top choice is the one above.:

38 minutes ago, crazy^millman said:

Parlec link: Link

Command: Link

 

  • Like 1
Link to comment
Share on other sites
1 hour ago, Bob W. said:

What is the control (Fanuc, etc...)?  Does it have DFO?  G54.2 I believe.

Fanuc 31i and I don't know if it has DFO, I'll have to look into that. What does it do?

There is already a hole/bore in the center of the table I was hoping to work with that but I would have to check if its accurately placed, It looks like part of the mounting mechanism.

We do use the twin boring head from Seco to rough and Sandvik devibe to finish, no drag marks allowed G76 boring cycle.

Link to comment
Share on other sites
10 minutes ago, Greg_J said:

Fanuc 31i and I don't know if it has DFO, I'll have to look into that. What does it do?

There is already a hole/bore in the center of the table I was hoping to work with that but I would have to check if its accurately placed, It looks like part of the mounting mechanism.

We do use the twin boring head from Seco to rough and Sandvik devibe to finish, no drag marks allowed G76 boring cycle.

Seco make good products also. Talk to your rep and see about getting an extension for the existing system to create the feature that allows you to get enough through it. I have done some 30" deep bores with a Twin bore and had no issues doing it.

Link to comment
Share on other sites

DFO (Dynamic Fixture Offset) is a control feature that uses two work offsets, G54 and G54.2, G55 and G55.2, etc...  G54 is for the center of rotation (COR) of the indexing axis and the other (G54.2) is for the part WCS position relative to the COR.  It allows for programming a multiaxis part away from the COR or if the part is programmed to the COR it allows for tweaking the position to reflect part setup inaccuracy.  If you set the part up and it was off by .1" in 'X' you could modify the G54.2 'X' offset by .1" and all of the indexed positions would be automatically calculated and updated by the machine control.  It works very well with probing but doesn't require probing.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites

I've only ever seen G54.2 with a P on a FANUC control. P1 through P8 are available.

There's basically a couple ways to do it. You can put your COR in the Common offset, then the X,Y, and Z distance from COR to part origin in your G54.2Pn offset. The other way is as @Bob W. Mentioned put your COR in your chosen Work Offset (G54, G55, G56, G54.1 P1, etc..)

  • Like 1
Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...