5th axis question

[bassn_07]

I will do my best to try and explain this as clearly as I know how. All the programs for our 5th axis has been programmed from the center of rotation and we use modular fixturing. Let's say if I needed to move a part onto another fixture and it was lower by a 1/4 inch, would I need to re post the program after transforming everything down or is there another way of doing it? Sorry if it seems like a silly question but I'm just trying to figure out the best way of doing things and this is the place to ask. Thanks again guys for helping my gimpy a$$.

[Fig sign]

The answer is yes ,repost after transform .

I always write my programs in incremental ,so every move I make takes me seconds .

If you have 300 absolute toolpathes I fell siorry for you

After transform and regen check carefully in backplot your toolpathes to be sure you moved everything properly .

HTH

[HEED]

It would be best to re-post it in my opinion cause you are working off of COR and that effects all your y positions as well as z and c. Re post it and make parts.

 

*EDIT*

DAM , Islander beat me to it, and yes inc. is better so that if you do have to translate your part, your paths and clearances follow...

[bassn_07]

Thanks for the reply. One quick question about incremental tool paths, why would incremental tool paths be any quicker then absolute if you need to transform and re post for both? Thanks again.

[gcode]

I have had very good luck with 3+2 type 5 axis

work and WCS..

I make a copy of Top and create a point to define Zero.

Like Iskander, all my toolpaths are incremental.

If I need to move things.. I just move my WCS point, regen and post..

Full 5axis stuff can bite you with this method..

I don't recommend it unless you have the ability to verify gcode

[HEED]

haha, now I was too quick to edit look up...

[HEED]

Wow, this topic is getting hit hard in the 2 mintes it's been up are you guys at work or are you eMastercam nuts at home too?

[bassn_07]

One more question regarding transforming, is there a quick way of transforming tool paths or does it all depend on how well the levels manager page is setup? The person before I didn't do a great job identifying his levels in detail.

[gcode]

It can be a real chore following behind

someone who doesn't label stuff.

Here's a neat trick that came out in X2..

Turn all your levels on..

Select an operation and click the icon

that looks like a circle and square in th Ops Manger.

Everything not associated with that op will be hidden..

You can use this to find move and organise

toolpath geometry, even if you've got hundereds of level full of unlabeled geometry..

[Fig sign]

Open all levels .

Select al entities

That`s what I do.

The worst part is when you rotate or mirror the part

You need to change cplanes ,chains directions ,

and chain sides on some of toolpathes .

Try to avoid it

 

BR

[bassn_07]

How is the center of rotation defined in Mastercam. I've been using startup programs to program a few simple parts where the modular fixturing is already established in Mastercam. God...I feel stupid for asking these question but I figure it's the fastest way to learn. Thanks again guys.

[Guest CNC Apps Guy 1]

CL Rotation isn't really defined per-se. With 5-Axis Matsuura that I program in Mastercam it does not matter. CAMPlete handles that stuff. But, if I'm using a Mastercam post, I create a "seed" or "Template" file with a pallet and basically make that pallet match my machine; position-wise that is. Then build my fixture, part, etc... on top of that. This way your numbers in Mastercam should match your G-Code, as long as your machine matches your mastercam file, you should be good.

 

HTH

[bassn_07]

quote:

---

CL Rotation isn't really defined per-se. With 5-Axis Matsuura that I program in Mastercam it does not matter. CAMPlete handles that stuff. But, if I'm using a Mastercam post, I create a "seed" or "Template" file with a pallet and basically make that pallet match my machine; position-wise that is. Then build my fixture, part, etc... on top of that. This way your numbers in Mastercam should match your G-Code, as long as your machine matches your mastercam file, you should be good.

 

HTH

---

What I would need to do is if I was starting from scratch is to figure out the number from my machine to the top of the pallet and create that in MC with the matching Z number...correct?

[Guest CNC Apps Guy 1]

No, from the top of the pallet to the centerline of rotation on your rotary table... assuming you're using a rotary/rotary configuration. Is this a correct assumption?

[MIL-TFP-41]

There are other ways around this also, provided you are using a newer Fanuc/Siemens/heidenhien control.

 

quote:

---

originally posted by MMT-USA

Basically TCPC is an option from Fanuc that instead of feeding the control direct XYZ ABC machine coordinates, you instead feed it cutter location coordinates that are always relative to the part. The controller will make the necessary calculations on the fly to account for the effects of the part rotation.

 

Some maybe familiar with this on the Siemens control called Traori or RTCP.

 

Programs using this function in Type 2 are independent of machine kinematics and machine zero. This means if you change the location of the part on the machine you do not need to repost it. You can also use the same program on a machine with completely different kinematics since the controller will make the necessary calulations to adjust for this.

 

TCPC automatically adjusts the axis feeds to make sure that the feedrate of the tool is relative to the part. No need for Inverse Time Feed G93

 

The controller modifies the axis motion so the tool follows a straight line relative to the part avoiding linearization errors do to kinematics.

---

Very cool stuff.

 

I have also used Fanucs "Rotary table dynamic fixture offset" (G54.2) with alot of success. Basically it lets you put your X, Y & Z position error in a offset & the control adjusts for it.

[cobra95kev]

I just use transform toolpaths function. It works real well and only takes a few seconds and it doesn't matter if you programmed in abs or inc.

 

My two cents,

 

 

[Ralph@Faustson]

I agree with JMC I'm using TNC controls and define the part zero ( X Y Z A & C ) in the preset table and I'm ready to go. I used to program where we had to move the model... if the absolute clearance moves are not far enough away and you have to move the model in Z it could cause problems.

[Josh T™]

Not meaning to hijack but...

 

James,

What do you think about CAMplete? We've had issues with some of the surface paths... inverting on parallel paths and thinking a scallop is a 5 axis path for instance. Your thoughts?

 

Josh

[Fig sign]

if the absolute clearance moves are not far enough away and you have to move the model in Z it could cause problems.

~~~~~~~~~~~~~~~~~~~~

I have created my custom holders .

I have a folder where I keep them .

Every time I write new part I merge existing fixture or create the new one

So I know my absolute clearance moves value .

This stile of work helps me to check my toolpath -

in backplot I see if the holder touchs the fixture or not .

Before veryfy I boolian add my fixture and blank part into one solid and use it in verify .

I define my tools together with holder as a tool with a step in diameter and actual tool length .

So in backplot I see a tool as tool and the holder

I use custom levels file so everything set according to the level names and they are always the same one.

I know them by heart and tipe them in level bar without calling level manager .

I use tool libraries .

All set nice and helps me avoid crashes using only backplot and verify .

[Guest CNC Apps Guy 1]

Hey Josh,

 

Well, I've been using CAMPlete (and supporting our customers that use it) over the last year and a few months. I can honestly say I've not run into the Inverting Toolpath issue. I've done a large variety of parts also 3 axis toolpaths through 5. With that said, I REALLY like it. So many things I used to have to think about and consider when I program without it... don't have to think about that stuff anymore. I can basically program my part from any location and transform the toolpaths and rotate them into position with a few mouse-clicks. It can do things that just can't be done without SERIOUS file modification on the Mastercam file. For example, I have a MAM72-35V and a MAM72-42V. I programmed my part considering the 35V, well the 35V is booked SOLID for as month and I have to get something through. With only Mastercam... BIG problem. One is a B/C machine and the other is an A/C machine. With CAMPLete... a few mousclicks and voila, no problem.

 

Full machine simulation ON G-CODE. It's a great enhancement to Mastercam, or any CAM System really. I would never even consider programming a MAM without it.

 

JM2C

[Josh T™]

Thanks for the input James. We use it sometimes for our Hermle C400i with the TNC430. I've heard CAMplete doesn't have many issues with the 530i control but our case is a little different. I love the transforms also!!! Mouse click and you can move the part around where you want it. The 3d verification is cool and probably easier than vericut. I was just wondering if you've had and surface machining issues.

 

Thanks again,

Josh

[kccadcam]

quote:

---

Well, I've been using CAMPlete (and supporting our customers that use it) over the last year and a few months. I can honestly say I've not run into the Inverting Toolpath issue. I've done a large variety of parts also 3 axis toolpaths through 5. With that said, I REALLY like it. So many things I used to have to think about and consider when I program without it... don't have to think about that stuff anymore. I can basically program my part from any location and transform the toolpaths and rotate them into position with a few mouse-clicks. It can do things that just can't be done without SERIOUS file modification on the Mastercam file. For example, I have a MAM72-35V and a MAM72-42V. I programmed my part considering the 35V, well the 35V is booked SOLID for as month and I have to get something through. With only Mastercam... BIG problem. One is a B/C machine and the other is an A/C machine. With CAMPLete... a few mousclicks and voila, no problem.

 

Full machine simulation ON G-CODE. It's a great enhancement to Mastercam, or any CAM System really. I would never even consider programming a MAM without it.

---

I had my first experience with Camplete today,,,

for our pair of MAM72-63V's.

I also had the honor of meeting CNC Apps Guy today.

(He looks way different without the glasses)

This is great software from what I've played with so far. The only shortcoming I see is no way of importing more detailed tooling info from Mastercam. (we'll figure out a solution, just getting into tool libraries here at my new job.)

The machine simulation motion is very smooth,,,

it even shows the way covers expanding and contracting!!

 

This is gonna be fun!!!!!!!

[Jayson Kramer]

James told me yesterday he was going to Oregon for some training but did not mention he going to see you Kevin.

Well I know he coming back to hang with us on Friday.

James should be taking picture with us and posting here. Wait! we need to get him a real bennie hat first.

 

James knows all ready but good people.

[MIL-TFP-41]

quote:

---

This is great software from what I've played with so far. The only shortcoming I see is no way of importing more detailed tooling info from Mastercam. (we'll figure out a solution, just getting into tool libraries here at my new job.)

---

In Camplete you can load tools into your toolchanger...so when you import your .nci file they are already there & defined.

 

Wait till you see the new version (I got a peek at IMTS)....very cool things are coming in the future.

[kccadcam]

quote:

---

In Camplete you can load tools into your toolchanger...so when you import your .nci file they are already there & defined.

 

Wait till you see the new version (I got a peek at IMTS)....very cool things are coming in the future.

---

Starting to populate tools into libraries, a little at a time.

 

Can't wait for the new stuff!!

CAMPlete is amazing software, it's so easy to get what you want....and know it's right.

This is the way Mastercam should build their posts,

the GUI interface is very easy to tweak.

You also "see" the G-code before it actually posts.