better control of lathe DOC...

[littlerob]

Do you people ever randomly need to turn on semi-finish because DOC V finish allowance is too much?

 

Question for the experts is; Is there an easier, more consistent way to control that?

 

My DOC is determined by Insert size, Horsepower and material. Not MC.

 

R

[crazy^millman]

I am sorry #1 no expert, but #2 that is not making sense. Need to turn on semi finish allowance? I have never used it, but have done a semi finish using a finish toolpath. I do that because I am extremely picky about how I name my operations. If I am roughing to +.100 then I say that in the Comments to be posted out with that operation. I don't want to confuse someone saying Roughing +.100 then Semi Finish +.05 with the same tool. the other issue is  normally rough with a WNG or CNMG stye tool and that might not get the semi finish I really want on a part with undercuts or other features where a DNMG, VNMG, Grooving or other others tools would. Then I might semi finish with a DNMG +.05 allowing it to get to places that I know a CNMG or WNMG would not. I then realy have confused the person running the job saying I am roughing to +.1o SEMI Finish +.5 with the larger angled tool to then come back and do the same thing with the DNMG tool. The other issue is depending on the Material I never want to just skim it with a tool. Turning is completely different than milling. Spring passes in Milling do create the same friction and cause material work hardening that happens with turning. I want my turning tool that would be doing SEMI finishing to take constant and consistent amounts of stock. By doing what I could with one tool then coming back and chasing it with a different tool I could create hard spots in the material defeating the purpose of doing the SEMI finish in the first place.

Glad your DOC process considers those things, but sometimes those things don't tel the full story.I have a 22" long shaft that is 1" starting diameter with 18" being turn downed to 1/4" if I went by that thought process only it may not work. I might need to approach it different depending on the machine the ability to use a follow or steady rest. Might want to rethink those kind of comments it shows a lack of experience doing this. It should be considered and help make the decision, but so many other factors go into what we do that broad statements like that are ways to easily trap yourself into not considering all things that go into Machining the part. Not trying to pick your thought process apart and again no expert, but after 35 years of doing this I have done enough stupid things to try to help others not repeat them. Remember there is much art and creative freedom as their science in everything we make. The end results should always reflect our personalities and have our personal touch on it.

[littlerob]

Thanks for the reply. I wasn't trying to sound confused, it just happens when I am. Disregarding the semi-finish info in my OP, I think that you probably acheive what I'd like to.

 

Basically if I tell the software I want to leave .025" for the finish pass, I end up with varying results. For example; today I left .025" for a finish pass, whilst taking .08" roughing passes. (No overlap, equal steps) but the result was much more. Something like .09" for a finish allowance. While I can work around this, it seems to me the stock left for finish shouldn't vary based on whatever variables. I'm quite sure this is oversight on my part, I don't know where. Thanks.

 

R

[littlerob]

After sleeping on it, I realized the topic title and content wasn't what I was after.....what I'm really asking IS about the finish allowance. It seems to vary for me, and I don't know why. I'd sure like to enter .025" in that field and it actually be that, every time. 

 

Some pics....

[crazy^millman]

The issue is you are using Equal steps and mis-understanding what and how that works. What would be the equal steps for one part may be the same for a different part, but seriously doubt it. Equal cuts is looking at the range you have defined. That is .08 max to .025 min so depending on the amount of stock to remove from the final shape that is big range for the software to determine what is the number of cuts and size to make each of them. I never use Equal steps because I learned long ago it is unpredictable and I like predictable process. This also means as much a you thought you were getting the optimal parameters for cutting the parts you were not. If that is the process you are going to be using then I can see where yes using semi finish in this case would be needed. I think it will not be as optimal as it can be, but that is where we have to experiment and try different things to see what gives us what we are looking for the best way.

In every Mastercam dialog there is the help button. I clicked on it and quoted from it. Learning what something does means reading about it and not assuming.

Quote

Rough Parameters

Use this tab to create a Lathe Rough toolpath. Compared to other types of Lathe roughing toolpaths, this tab offers you the most complete set of roughing options.

Enter your cutting parameters in the fields, and choose a cutting direction and select an orientation for the toolpath in the Rough direction/angle drop-down list. Use the pictures as a guide for entering the toolpath dimensions. You can also select cutter compensation and enable advanced features such as a semi-finish pass, lead in/out moves, and toolpath filtering on the right side of the tab.

../../../Skins/Default/Stylesheets/Images/transparent.gifParameters

Entry amount

Enter the distance from the stock that the tool starts to feed.

Exit amount

Specify the amount that the tool moves beyond the stock boundary at the end of a cut.

Cutting Method

Choose a cutting method/direction from the drop-down menu.

• One way: The tool cuts the part in one direction, comes up, goes back to the beginning, and cuts again. The picture in the dialog box changes to show this tool motion.
• Zig zag straight: The tool cuts the part in a straight back and forth motion. The picture in the dialog box changes to show this tool motion.
• Zig zag downward: The tool cuts the part in a downward back and forth motion. The picture in the dialog box changes to show this tool motion.

Rough direction/angle

Determines the angle that the tool cuts into the part. This angle is relative to the rough direction, OD, ID, Face, or Back.

Overlap

Select to create an overlap between each rough cut. Click to set how much the tool overlaps the previous cut before making the next cut. If deselected, the tool will not retract before cutting down to the next level. For canned rough toolpaths, you only enter the value.

Auto

Removes material equal to the Depth of cut during each pass, until the depth of cut value becomes too large and will begin to make smaller passes. Those passes will not be less than the Minimum cut depth.

Equal steps

Removes the same amount of material per pass without exceeding the Depth of cut value.

Incremental

Removes an incremental amount of material with each pass, starting at the Initial cut depth and increasing or decreasing until it reaches the Final cut depth.

Initial cut depth

Sets the initial cut depth of the incremental type of Depth cuts.

Depth of cut

Sets the amount of material to be removed during each cutting pass. This option is only available when Depth cuts is set to Equal steps or Auto. If Equal steps is selected, then this value determines the maximum amount of material the tool can remove per pass.

Increments of

When selected, Mastercam will cut the first pass at the Initial cut depth and then cut the following passes at the Initial cut depth plus the Increments of amount until the Final cut depth has been reached.

Only available when Depth cuts is set to Incremental.

Final cut depth

Sets the final cut depth of the incremental type of Depth cuts.

Minimum cut depth

Determines the smallest cut that can be taken per pass. Only available when Depth cuts is set to Auto or Equal steps.

Stock to leave in X

Determines how much stock remains in the X direction when the operation is finished. Typically, this would be removed by a separate finish operation.

Stock to leave in Z

Determines how much stock remains in the Z direction when the operation is finished. Typically, this would be removed by a separate finish operation.

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 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 cut.

• The passes will alternate between angled and straight.
• 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.

Compensation type

The options that are available to you are determined by the active control definition. Choose how you want to handle cutter compensation:

• Computer: Mastercam computes the compensated toolpath and does not output control codes for compensation. 
• Control: Mastercam outputs control codes for compensation and does not compute the compensated toolpath. 
• Wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same. 
• Reverse Wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
• Off: Mastercam programs the tool tip directly on the chained geometry and does not output compensation codes.

Optimize cutter compensation in control

Eliminates arcs in the toolpath that are less than or equal to the radius of the tool and helps prevent gouging. The default setting for this field is set on the Cutter Compensation, General page in the Control Definition.

This field is available only when Cutter compensation is set to Control on the parameters tab, and applies only to that setting.

Compensation direction

Choose to offset the tool to the right or left of the toolpath. Even if cutter compensation is set to Off, Mastercam uses this setting to determine the orientation of other toolpath features such as multiple passes.

Roll cutter around corners

Inserts arc moves around the corners in the toolpath. Choose the type of arc move:

• None: Guarantees all sharp corners.
• Sharp: Only rolls the tool around sharp corners of 135 degrees or less.
• All: Rolls the tool around all corners and creates smooth tool movement. The radius of the arc moves equals the radius of the tool.

This option is available only when Compensation in computer is turned on.

Semi finish

Select to create a semi-finish pass after the final roughing pass. This pass follows the contour of the part with the roughing tool, preparing it for the actual finish operation. Click to configure the semi-finish pass.

Lead in/out

Select to have Mastercam add lead in/out moves to the toolpath. Click to edit the moves.

Plunge parameters

Click to define how the tool handles undercuts on the toolpath along each axis.

Filter

Select to eliminate unnecessary tool moves in the toolpath to create smoother movement. Click to configure toolpath filtering options.

Tool inspection

Select to turn on tool inspection. If the checkbox is already selected, click the button to open the Tool Inspection dialog box and change the tool inspection options.

Chip break

Select to turn on chip break. If the checkbox is already selected, click the button to open the Chip Break dialog box, in which you can change the chip break options.

Section turning

Select to turn on Section turning. If the checkbox is already selected, click the button to open the Section Turning dialog box, in which you can set the toolpath to break into sections.

Stock recognition

Adjusts the area of the stock to be removed by the roughing operation. The following options are available:

• Remaining stock: uses only stock remaining from previous operations.
• Use stock for outer boundary: uses a section of the stock boundary as the outer boundary.
• Extend contour to stock only: linearly extends the ends of the chained contour to the stock.
• Disable stock recognition: provides no stock recognition.

Adjust stock

Opens the Adjust Stock dialog box and lets you adjust the area of the stock to be removed by the roughing operation. This option is available only if:

• You define stock boundaries in the machine group properties.
• The chained contour lies entirely within the stock boundary.
• You select either the Use Stock for Outer Boundary or Extend Contour to Stock Only options.

Shorten pass

Use to adjust the start of each pass based on the shape of the remaining stock from the previous pass and the shape of the tool.

Linearization tolerance

Used when converting 3D arcs and 2D or 3D splines in the chained geometry from curves to lines. Smaller linearization tolerance values make more accurate toolpaths, but may take longer to generate and create a longer NC program. This parameter is only available when chaining splines.

 

[littlerob]

Appreciated.

I have tried using "Auto" and "Incremental". I get similar results ..it seems that the only way I can get the finish allowance of .025" consistently, is changing my Rough depth cuts to something close to .025. Fore that is not optimal. I read through your post and the help dialoge, but you didn't say which parameters you use exactly...maybe what you're doing is what I need to do.

[crazy^millman]

49 minutes ago, littlerob said:

Appreciated.

I have tried using "Auto" and "Incremental". I get similar results ..it seems that the only way I can get the finish allowance of .025" consistently, is changing my Rough depth cuts to something close to .025. Fore that is not optimal. I read through your post and the help dialoge, but you didn't say which parameters you use exactly...maybe what you're doing is what I need to do.

I have always used Auto with a Depth of Cut. Again to get what you are after I have used a Finish pass set to the amount of stock I want to leave and I think you want it al done in one operation and to do what yes you will need to use SEMI Finish in the operation to get what you are after.

[gcode]

We use separate chains for roughing, semifinish and finish

Stock to leave is always zero on all toolpaths

It's more work but it is 100% reliable and you never screw up a part because 

"Stock to Leave" was set incorrectly

[AHarrison1]

Something else worth trying is turning on overlap...

With overlap on I get the .025" gap

 

With overlap off the gap is approx .085"

[BBprecise]

I haven't done much lathe programming lately, but when I do need to rough the part I use the roughing cycle and it always leaves me the correct amount of material. Always. Using equal steps tells Mastercam I want the doc's to be as close to this amount as possible but I also want the doc's the same amount. If you're getting to much material left on reduce your min. cut depth. I have Mastercam set my default at .015" and I can't say I've ever noticed it not leaving the right amount w/in a couple thousandths anyways. If The finish tolerance is +/-.005 or more I don't care about a few thousandths extra. Tolerance down to +/-.002 then do 1 sizing pass and a couple extra thousandths on the 1st pass won't change cut diameter noticeably. Tolerance tighter then +/-.001 and we do at least 2 sizing cuts and a few thousandths wont bother here either.

Now when cutting Inconel, Rene, Titanium and some hardened ph series stainless (only if we cant control the time/length in cut good enough with a general roughing cycle) we create geometry for every depth, but only to control the time in cut and the entry/exit method so we don't leave sharp corners that with notch a ceramic insert in Inconel and Rene instantly.