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:

Lathe Tips and Tricks


Colin Gilchrist
 Share

Recommended Posts

This is how I do it ...

 

1-2.png

 

 

 

2-2.png

 

 

 

3-1.png

 

 

 

4-1.png

 

 

 

and I get this code...

 

 

N1

(T1 | OD ROUGH RIGHT - 80 DEG. | ID CODE - 1.)

(TOOLPATH GROUP - TOOLPATH GROUP-2)

G123.1

M901

M202

G53.5

T1.01 M6

G28 U0. V0.

G28 W0.

M250

G0 B45.

M251

G53.5

G18

G50 S6000 R1

G96 S200 M03 R1

G0 X10.14142 Z.07071

G99 G1 X10. Z0. F.01

X0.

Z.1

G28 U0. Y0.

G28 W0.

M05

M01

M30

 

At least I think that is what you are after. :thumbsup:

Link to comment
Share on other sites

[At least I think that is what you are after.]

 

 

 

You read my mind.I want an M04 so I used a Left-164 tool and rotated it B180, comp right ( code and backplot) looked good.I guess it was straigt forward.Curious how to make this less redundant.Do I modify and save the default setting for face and turn ops or modify the post (rather not)?How did u get the T01.01?That would be nice.

Link to comment
Share on other sites

I noticed the post added a G28 home move and repeated the work coor along with a B axis move(doesnt happen with rotation box left alone)for the turn move after facing.If I left the B rotation out (accidently because Im human)the B axis defaults to 90 deg.(not good)I tried to edit tool permanently but .

 

 

 

 

 

(PROGRAM NAME - T DATE=DD-MM-YY - 23-04-12 TIME=HH:MM - 15:43 )

(POST LICENSE - IN-HOUSE SOLUTIONS INC.)

(T1 | MCMNN- L-164C - CNMG-432 | DIA. - 1 | SUFFIX - 1. | INSERT - CNMG-432)

G20 G69 G80 G40 G18 G90 G94

M205

(T1 | MCMNN- L-164C - CNMG-432 | DIA. - 1 | SUFFIX - 0. | INSERT - CNMG-432)

(TOOLPATH GROUP - TOOLPATH GROUP-1)

G20 G10.9 X1

N1 G91 G30 P3 X0.

N1 G30 P3 Y0. Z0.

M901

M202

T1.01 T1 M06

G91 G30 P3 X0. Z0.

G90

M108

G0 G90 G53 B45.

M107

G54

G90 G43 P1 X4.278 Y0. Z0. H#3020

G18

M239

G92 S6000 R1

G96 S500 M204 R1

G95 G1 X-.0625 F.01

G91 G28 X0.------here

G28 Y0. Z0.

G90

T1

G54------here

M108

G0 B45.----- here

M107

G0 X4.078 Y0. Z0.

Z.1

G1 Z0.

Z-2.3238

X4.2194 Z-2.2531

M205

G91 G28 X0.

G28 Y0. Z0.

G90

M30

Link to comment
Share on other sites
  • 1 month later...

I've noticed the views on this topic going up, but nobody posting. Feel free to post your own tips, or as questions if you have them.

 

I was give a big list of other Tips/Tricks with Lathe by some of the Developers here at CNC, I've just been so busy I haven't gotten a chance to post them yet. More to follow...

Link to comment
Share on other sites

Time for an update.

 

When creating a new Lathe Tool, the Lathe Tool Setup dialog box will show how the tool is loaded Graphically.

 

LatheToolSetup.png

 

In the Lathe Tool Manager (or in the Tool List in an Operation) the graphics will indicate the insert direction. The Inserts shown in Orange are defined as "Insert Down" and the yellow inserts are defined as "Insert Up".

 

LatheToolPictureopsmanager.png

 

Sometimes with ID work there is very little clearance between the Tool/Holder and the part. This can cause a false collision warning if the tool is too close to the part. In that case you may need to reduce the entry/exit clearance in the Lathe Stock Update dialog, located in the Lathe Operation Parameters.

 

StockUpdateParametersLathe.png

 

It’s common for a lathe holder to support multiple inserts, for example different corner radii. Our tool catalogs contain most of the holder/insert combinations, but not all of them. In that case, you can define your own tool by selecting the holder from a holder catalog, and the insert from the insert catalog. You can even combine a lathe metric insert with an inch holder, or a lathe inch insert with a metric holder. Remember to save these custom built tools to a Lathe Tool Library for future use.

Define Tool:

DefineLatheTool-InsertPage.png

Inserts:

LatheInsertLibraryDialog.png

 

I've uploaded an example file to the FTP site. It is named "RIGHT HAND VS LEFT HAND - PCLNR3225P12-R08.MCX-5" and is located in the "Lathe" sub folder.

 

When you are setting up a new Lathe Tool, I recommend you use the "Draw Tool" button on the "Define Tool" dialog box. This will draw a wireframe representation of your tool, and will show you the clearance angles that are setup for that tool (indicated by the red and purple circles). If the orientation of the tool looks correct on the screen, then the tool is properly setup.

 

Let me know if anyone has questions about creating a Lathe Tool and I'll provide some follow-up information.

Link to comment
Share on other sites

Does anyone here using Sandvik Coromant "Twin Tools" or even their Corplex MT combined Milling and Turning tool? If so, I'd be curious to see how you set up and apply these in Mastercam.

 

These reply on the M602/603 commands (on the Okuma Multus) to orientate the tool to use (for example) the CNMG insert, or the DNMG insert.

 

The Coroplex MT is tricky, as it is a R390 two insert endmill, and a CCMT and DCMT turning tool combined. :)

Link to comment
Share on other sites
When in VTL mode if you want to make your dimensions display in the orientation you would expect you need to make a new construction plane. Go to Planes, planes by geo, pick a horizontal line, then a vertical line. X should face right, Y should face up.

Save that new plane as a unique name "drafting".

 

That works or just click on Planes = Gview

Link to comment
Share on other sites
  • 2 weeks later...

I discovered a new trick. To quickly chamfer an edge on Lathe rough face or turn, (I was facing), shorten the contour in lead in/out by the desired chamfer amount (.05x45), in add line, set length to .05, angle to 45, leave overlap on but set value to 0, and uncheck equal steps. Sounds like a lot, but it adds a quick chamfer during roughing.

Link to comment
Share on other sites

I discovered a new trick. To quickly chamfer an edge on Lathe rough face or turn, (I was facing), shorten the contour in lead in/out by the desired chamfer amount (.05x45), in add line, set length to .05, angle to 45, leave overlap on but set value to 0, and uncheck equal steps. Sounds like a lot, but it adds a quick chamfer during roughing.

 

That is a good one.

 

The Lathe Face toolpath has 'Corner' options that allow you to optionally chamfer or radius your part. Lathe Finish also has the 'Corner' option to allow you to chamfer/radius your geometry. The only bad thing about using the Lead In/Out to cut the chamfer for you is that you loose some control over the retract motion, and you are limited to only being able to cut the first and last piece of geometry in your chain.

Link to comment
Share on other sites

That is a good one.

 

The Lathe Face toolpath has 'Corner' options that allow you to optionally chamfer or radius your part. Lathe Finish also has the 'Corner' option to allow you to chamfer/radius your geometry. The only bad thing about using the Lead In/Out to cut the chamfer for you is that you loose some control over the retract motion, and you are limited to only being able to cut the first and last piece of geometry in your chain.

Im using Lathe Rough with stock rec. I haven't used lathe face much, I'm not facing to center, and I did not see tool inspection in lathe face. Retract is working fine. I'm just pre roughing a part, quicker then drawing chamfers. It does just cut the chamfer at the end.

Link to comment
Share on other sites
  • 1 month later...
  • 4 weeks later...

Thought I'd add something else to this thread.

 

Cutoff Toolpath

 

Starting in X5, there was an option added to the 'Stock Update' parameters for handling the Stock definition after a cutoff operation. Prior to X5, the only available options were 'Keep separated piece' and 'Keep piece in active chuck'. With X5, a third option for 'keep both pieces' was added. This allows you to create the new piece of stock in the sub spindle, and keep the remaining stock in the main spindle. (This more accurately represents the process on the machine)

 

POCO

 

If you use the new Pickoff/Pull/Cutoff Toolpath in X6, the Cutoff operation is added to the sequence of Chuck events that allow you to configure and backplot the entire stock transfer process. When you run the POCO utility, there are several "strategies" that you can choose: Pickoff only (basic stock transfer between spindles), Pickoff/Cutoff (prepositions the cutoff tool, approaches and clamps on the stock with the sub spindle, cuts off the part, retracts the sub spindle), Pull (uses the sub spindle to perform a bar-pull operation), and Pickoff/Barpull/Cutoff (prepositions the cutoff tool, approaches and pulls the stock, cuts off the part, and retracts the sub spindle). When you take the time to configure the toolpath options in the utility, these parameters are saved to a parameter file, so your choices are remembered the next time you run the POCO utility.

 

There is a document; X6 Pickoff/Pull/Cutoff Applications Guide, that is available through your Mastercam Reseller. It describes how to use and configure POCO and modify your Post Processor to process these toolpaths. The download for this guide also contains sample MCX-6 files that will work with the 'Generic Fanuc 4X MT_Lathe' post processor.

 

Plunge Turn Toolpath

 

X5 also saw the introduction of the Plunge Turn toolpath. This toolpath currently only supports 'Flat bottom' style inserts, but enhancements have been requested to support other tool types.

 

Variable Cut Depth option in Roughing

 

Not sure if I mentioned this feature previously, but X6 now supports variable depth cuts in the Lathe Rough toolpath. From the help file:

 

Variable depth

Allows you to vary the point that the surface contacts the tool insert to prevent notching and improve tool life. The variable depth can vary up to 25% of the depth of cut. The actual depth of cut can vary from 75% to 125% of the normal depth of cut. The valid range is -25% to +25%. A positive value will result in an upward cut and a negative value will result in a downward cut. Zero will result in a straight (normal style) roughing cut.

 

Notes:

  • The passes will alternate between angled and straight (after the variable depth pass, a straight pass is added to cleanup that "cut")
  • If the cut length is less than three times the cut depth, a straight cut will be made instead of an angled cut.
  • In flat areas, a straight cut will be made instead of an angled cut.
  • One way and zig zag cuts are both supported, as well as ID, OD, Face, Back, and Angled.

Link to comment
Share on other sites
  • 2 months later...

Hi Wes,

 

Unfortunately I'll have to wait until X7 is officially released before I can show anything from MT, or the enhancements to regular Lathe. I could start a thread in the Beta forum to discuss/document this stuff, then just copy it over once X7 is released.

 

I know setting up tools for MT will be a good feature to document, especially with the Tool Angle functions for controlling the B axis head, and the A axis angle (for rotating a tool from main spindle to sub spindle). There is also some great new functionality for automatically setting Axis Combination/Toolplane, based on the type of path you select.

 

I am planning on starting a new thread on creating POCO (Pickoff/Cutoff) operations. That will be a new thread because I'm also going to document how to modify a post to process the POCO NCI events properly.

 

Thanks for the feedback!

 

-Colin

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...