52 replies to this topic

[Colin from CNC Software]

I wanted to share some tips that Lathe users might find useful.

Deleting Stock

I found something that I thought was really useful the other day. I was working on a lathe file that had a Stock Transfer operation. I needed to modify one of the operations on the Main spindle. When I did that, I kept getting errors with Stock Collisions during regeneration.

I think the reason for these collisions has to do with Stock Recognition for Lathe. If one (or more) of your operations use stock recognition, the algorithm expects there to be some stock remaining for the toolpath to cut. Because the stock has been 'Transferred' to your other spindle, Mastercam expects some stock to exist, but doesn't find any.

The solution I found was to go into Stock Setup and delete both the Left and Right spindle stock. Then redefine the original stock in the left spindle. If you do this, you should be able to change anything you want, then regenerate all your operations from the start without problems. I tried this on a bunch of different files, so I'm hoping it will help someone who has encountered this before.

Use the Back Toolplane

For Lathe, C zero is referenced from the 'Back' Toolplane in Mastercam. With the Back Plane, X+ points towards the Chuck (left) on the Main Spindle. The only operations that do not reference 'Back' as C zero are 'Axis Substitution' type toolpaths, which must use Top for the Toolplane. Due to a quirk of how the planes are defined though, you will get a 'mirrored' image on the machine. You must draw the shape in the 'Bottom' plane, then toolpath in the Top plane for proper output.

When creating Toolplanes for Mill Toolpaths, always start by setting the active plane to 'Back' then rotate the plane around the X axis. This will ensure that you get the proper C angle.

Start fresh with an X6 Lathe Post

Starting with X4, some significant work has been put into our Generic Lathe Posts (specifically Generic Fanuc 4X MT_Lathe.PST). Improvements include new handling of Cutter Compensation for Lathe Canned Turning/Grooving toolpaths, modifications to 'pstck_trans$' and 'pchuck$' for the new Cutoff/Pickoff/Barpull utility, improvements to Arc Break routines and sweep$ handling routines, and much more.

If you've been modifying the same post from an old version of Mastercam, it might be time to consider an upgrade.

Please feel free to post other Tips and Tricks you've learned when working with Lathe. This isn't a thread for complaining about problems, we have plenty of those threads already.

Thanks,

[Wes@M.A.D.]

Colin, try some of these and let us know what you come up with

Deleting Stock
What about syncronized turning? I do a lot of that. The part is mounted in both spindles. I have turning on the main side using upper left axis combo's. I also have turning on the sub spindle using upper right axis combo's. I amost always get stock colision's. I also use, lets say a CMNG-432 as tool 1. If I program a path at the main and then pivot the tool 180 (like the machine does)to program at the sub I get errors and have to create a new dublicate tool.


Use the Back Toolplane
this works fine for most lathes. We have the older sytle Integrexes that use the C zero pointing to the back as you say. We also have the new Integrexes (E) and (I) that have C zero pointing up as it does in a vertical Mill. This also will cause problems

Dont get me weong,I know how to make all this work, but I was curios of yoour thoughts

Thanks

[Colin from CNC Software]

Wes@M.A.D., on 13 March 2012 - 09:24 AM, said:

Colin, try some of these and let us know what you come up with

Deleting Stock
What about syncronized turning? I do a lot of that. The part is mounted in both spindles. I have turning on the main side using upper left axis combo's. I also have turning on the sub spindle using upper right axis combo's. I amost always get stock colision's. I also use, lets say a CMNG-432 as tool 1. If I program a path at the main and then pivot the tool 180 (like the machine does)to program at the sub I get errors and have to create a new dublicate tool.


Use the Back Toolplane
this works fine for most lathes. We have the older sytle Integrexes that use the C zero pointing to the back as you say. We also have the new Integrexes (E) and (I) that have C zero pointing up as it does in a vertical Mill. This also will cause problems

Dont get me weong,I know how to make all this work, but I was curios of yoour thoughts

Thanks

Synchronized turning isn't really supported in the current version of Lathe. Is it possible to just define the stock in the Left spindle and use only that stock definition, but define both left and right chuck? I tried it and it seems to work ok.

Regarding the Tool: You can define a Tool in the Upper Left Axis combination that can cut on both spindles. In order for this to work, your Machine Definition needs a 'Lathe B Axis Arm' added to the Upper Left Tools group. In the properties for the 'B Axis Arm', set the axis of rotation to 'Z'. Then make sure the B Axis Arm is included in your Axis Combination.

By adding the correct 'B Axis Arm' component, you will now have the 'Tool Angle' button available in the Toolpath Parameters. This lets you flip the Tool 180 degrees (without having to define a duplicate tool) so you can work on the Right Spindle.

For a Mill/Turn machine with a different C Axis zero position, you would either have to rotate your geometry properly (it would appear rotated 90 degrees in Mastercam) or you need a post that will manipulate the 'rotaxtyp$' variable, and will then calculate the angles correctly. Either solution presents a challenge.

[Wes@M.A.D.]

thanks Colin

Quote

Synchronized turning isn't really supported in the current version of Lathe

hope this is getting addressed, need to keep up on that technology that has been around for some time now  

[K2csq7]

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".

[Colin from CNC Software]

I can't comment on future versions or enhancements that aren't in a released product. Let's try and keep this thread on using X6 Lathe.

If you do have suggestions for enhancements, please send them to QC@mastercam.com.

Thanks,

[Colin from CNC Software]

While I understand there can be frustrations, that isn't what this thread is about. There are plenty of other threads to ask questions or voice your displeasure.

Let's try and keep this thread on-topic.

Thank You.

[K2csq7]

If you want to change your feedrate in the middle of the toolpath, but don't want the "toolpath editor" to lock up your operation.
Open the geometry box, right click on your chain & choose "change at point". The changes will stick even through a regeneration.

[Colin from CNC Software]

If anyone machines HRSA (Heat Resistant Super Alloy) steels, you can use the new 'Variable Depth' feature in the Lathe Rough Toolpath to vary the depth of cut. The 'Variable depth' field accepts values from -25% to +25%. This -+ value tells the toolpath to either plunge or retract along the cut, as a percentage of the 'Depth of Cut' value. After the 'variable' cut, the next cut is a straight cut (which also varies the depth during the cut, as the stock thickness changes).

The end result is a toolpath which reduces 'notch' wear on your inserts. This strategy is especially important for ceramic inserts.

[Jeremy Herron@DBS Solutions™]

Another trick for HSRA materials is in your leadin/out tab shorten your contour your stepover amount + the amount of stock you want to leave, for example your stepover is .03 +.01 stock to leave =.04,  and use the entry/exit arc set to .04  to effectively "roll" in and out of the cut. Great for tool life.

[Jeremy Herron@DBS Solutions™]

Down cutting allows you to finish faces and diameters in one tool path, instead of having to finsih the faces in one toolpath and the diameters in another.

[Colin from CNC Software]

My Tool crashes when trying to regenerate an operation. What's going on?

I see this often when a user starts programming a job on the left spindle, then programs a stock transfer. Initially, the user only defines Left Spindle stock/jaws. Then defines the Right Spindle when creating the stock transfer. Afterwards, they try and modify one of the left spindle operations and get warning about the tool crashing into the stock/chuck.

The solution is to check the Home Position for the operation that is giving you problems. Depending on the XZ home position, Mastercam thinks your tool is going to hit either the stock or the chuck during the move to/from the tool change position. To solve this, I usually set Home Position to 'user-defined' and use the select button to pick a point outside of my chuck boundaries. This should allow you to regenerate without any collision warnings. (you may also need to delete and re-create your stock definition as mentioned earlier)

[Colin from CNC Software]

Anyone can feel free to ask "how do I" questions or post tips and tricks of your own. I just didn't want the thread to get cluttered with 'non-help' comments.

[CADCAM3D5AXIS]

Hi Colin
How do you  speed up the regerate tools setting after an op goes dirty so the comp does not drag like it is stuck in the mud until it goes thru all the cuts that are dirty ??

[CADCAM3D5AXIS]

Hi Colin
How do you  speed up the regenerate tools setting after an op goes dirty so the comp does not drag like it is stuck in the mud until it goes thru all the cuts that are dirty ??
And are there config settings that will make this stick!
TIA

[Colin from CNC Software]

CADCAM3D5AXIS, on 12 April 2012 - 11:01 AM, said:

Hi Colin
How do you  speed up the regenerate tools setting after an op goes dirty so the comp does not drag like it is stuck in the mud until it goes thru all the cuts that are dirty ??
And are there config settings that will make this stick!
TIA

I'm not sure what you mean? Are you saying the regeneration of the toolpaths is very slow? I would think this has more to do with the computer hardware you are using, especially your graphics card.

I just did a test on a Lathe file I'm working on. 126 operations. I changed the origin for my right spindle Toolplane by .01 in Z, which caused about 50 of my ops to go dirty. I regenerated the dirty ops in under 10 seconds.

Does this delay happen on all your Lathe files? Does the number of operations in the file seem to make a difference?

I'd recommend sending a file to QC[at]Mastercam[dot]com and see if they can offer any insight.

[CADCAM3D5AXIS]

Hi Colin  
WHEN i do the regenerate to clean up a op after a edit the process time goes really slow. After it does this it moves like it should after it goes thru one re gen. it happens every now and then but it is a pain when it has to sit thru this.also at the task bar on top of the Mcam window during the regen it says not responding while its drawing the toolpaths and not leaving a clean screen during this op.but it cleans up after it plows thru whatever its doing. Is there some Optimum settings for the verify / regen settings that i should have a s a default settings.
Thanks

[gcode]

The new facing options in X6 are slick.

Now you can radius or chamfer the an OD with a facing toolpath

There are even various options for roughing the radius or chamfer
good stuff

[Jeremy Herron@DBS Solutions™]

Another HSRA trick for roughing grooves and undercut geometries, create a 2d highspeed mill toolpath to cut Dynamically rough the groove using the ziz zag method, backplot and save as geometry, You can use this as a chain for a dynamic turning toolpath. Works great with ceramics and carbide round inserts as you get to roll in and and out of the cut, use both sides of the insert, and eliminate unnecessary moves.

[newbeeee]

^^^neat Jeremy