Mastercam Turning
Rosita Westhouse
Anyone have any experience with custom tools in MasterCam lathe 2018? I'm trying to create a back-turning tool. I drew a .125 wide back-turning tool (Sandvik Corocut xs #MABR 3 020 125) but I'm having issues with the toolpaths. I can cheat and make it work by adding a couple of lines and creating a groove on my part but I would like to get it to work like a standard turning tool.
I don't have a solid of the tool. I drew it in mastercam based on measurements I took of the insert. I am using Lathe 2018. I should point out that I am using lathe default but for a Citizen swiss lathe. I draw on the right hand side to get "Z" moves in the plus direction which is how Citizens are set up.
So I created the tool based on a training tutorial I found online, I believe its from Mastercam. They have you draw a tool on level 111 then from the lathe tool manager you "create new tool" "custom" then enter the geometric tool orientation, tool geometry, tool orientation in turret, corner radius, tool center, and compensation.
Not the best way to do it in my humble opinion. Take an existing tool and then in the lathe tool manager right click and save to level use that to help you road map what your after. Too many ways to make mistakes staring from scratch. By using an existing tool you have a much better chance to get it correct. Then use that new level tool to make the custom tool and I think you will be golden.
So I was able to create the tool no problem with the method above but I'm having a similar problem as before where I get a "Toolpath starts with the tool embedded in the stock" error. By changing some setting in the tool path I can get it to run through put then the tool cuts in places it should not.
Here is some pictures of whats happening and how the tool is setup. In the picture of the part the yellow line is what I want to back-turn, the blue line is where it's going to which is above where I want to make a finish path. I will post the other pictures separate, it won't let me post all of them together.
Finally got it to work. Took a little experimenting but after turning off the stock update and playing around with orientation as stated above its cutting as it should. Posted code and that looked good too. Needed to change the orientation in both top plane and turret to #6. Thank You!
I am so sick and tired of Mastercam's mill turn and trying to get my DMG Mori NTX2000 to work right. There are so many damn hand edits and it is risky (editing mistakes) and time consuming. These aren't custom features, they are things like unclamping the B-axis for 5-axis machining and getting the G68.1 to post correctly. Things that EVERY NTX 2000 CAN DO!!! CNC Software, why the hell doesn't this xxxx work? You are wasting my time! The cost of my lost productivity far out paces the cost of your mill turn product. You owe it to me to fix this crap and deliver a product that works. I paid for it, now deliver. If I had access to the post I could fix all these issues in a matter of hours, not months or years.
I was reading in the mill turn application guide for the Mori and it calls out the correct format for G68.1 pattern 1 but the posted code isn't output correctly, LOL! Actually I don't think it is funny at all, I feel like a sucker that is being screwed after buying a product that doesn't work and is costing me $xx,xxx in lost productivity. I bought Esprit but I REALLY want to stick with mastercam because that is what I know. I just needs to work...
Yeah, programming in mill-turn really is a piece of cake. The challenge is every program with a new feature (cutoff/ pickoff, TCP, G68.1, etc...) never runs right on the machine and results in calls with our dealer, calls with Mori, etc... We identify the issue and have to hand edit every program. I feel like my mill turn post is the prototype.
Working with my reseller. They have indicated frustration at having to make the same changes over and over because the base posts at CNC aren't getting updated. The Mori AEs warned me about this and told me other shops in the area spent months trying to get Mastercam working correctly before giving up and switching to Esprit. My thought was all that work couldn't have been for nothing and the issues surely made it back to CNC and the posts were updated but I was clearly wrong and the AEs were right. It has played out pretty much as they said it would. At this point all I can do it put the word out so someone trying to decide between Esprit and Mastercam knows what they are in for.
I can certainly see both sides of this, much of MCs "bad" rep has come from messed up posts (MP) floating around out there which generate bad code which is then blamed on MC. I am sure this is frustrating for CNC and so it isn't surprising to me that they want to keep more control of MT.
The post for my machine was the latest version downloaded from Mastercam so these issues are baked into that version. I think unclamping the B-axis for 5-axis machining is one of the issues my reseller has to deal with over and over, among others. B-axis contouring is specified with M594, then is needs to be unclamped with M369. Well the M369 isn't posted so the machine hangs up. If Mastercam worked I feel it would be a much better product than Esprit but I am also a little biased because it is what I know. If it doesn't work it is kind of a moot point though. I haven't even started thinking about implementing some of the custom technology cycles yet. Just getting the machine to run a basic program without edits is challenging enough.
FWIW, we are a 5-axis aerospace shop running Makinos and the Mori NTX. We are AS9100 certified and ITAR registered. We make rocket and fighter jet parts and we are good at what we do. I really need my tools and equipment to work so we can do our jobs and keep our customers happy. I hate it when faulty tools or equipment make our job harder... We already have enough challenges to deal with in just making the parts we make.
Shouldn't be that bad. We have a bunch of customers with that type of machines and it's usually pretty smooth sailing after few weeks...most of the time it's just a matter of training. Jay K and Bill M might be great contacts at CNC Software for those types of issues IF it comes to training?
We have to work to hold .001"... On our Makinos we comp a tool, walk away, and hold .0001" all day long. We can hold .0005" (.7500" +0/ -.0005) on long cylindrical bores using a ramped toolpath with a lollypop mill and .0003" circularity. No can do on the Mori, I was spoiled.
Here is an example of an issue that isn't yet fixed and has given us a lot of grief. We were drilling a skewed hole on the NTX and the drill wasn't going to the correct position by about 1/2". We had other G68.1 issues in the past but we came up with quick fixes such as surface machining a skewed face instead of face milling it. The issue was the machine and Mastercam are set to diameter for both upper and lower turrets for milling AND turning but Mastercam was posting in radius coordinates during G68.1 plane rotation. When doing plane rotation the machine needs M-codes (M582) to put it in radius mode. Once those were hand edited in it worked flawlessly. Still waiting for the post fix however.
Here is an example of an issue that isn't yet fixed and has given us a lot of grief. We were drilling a skewed hole on the NTX and the drill wasn't going to the correct position by about 1/2". We had other G68.1 issues in the past but we came up with quick fixes such as surface machining a skewed face instead of face milling it. The issue was the machine and Mastercam are set to diameter for both upper and lower turrets for milling AND turning but Mastercam was continuing to post in diameter coordinates during G68.1 plane rotation. When doing plane rotation the machine needs M-codes (M582) to put it in radius mode. Once those were hand edited in it worked flawlessly. Still waiting for the post fix however.
Another annoying issue (not post related) is we were boring a large part with a lip on the ID of the front of the part (think 6" diameter coffee can with a 3" hole through the lid). We got the correct tool for this but it caused X-axis overtravel issues with the lower turret. We flipped the tool over 180 degrees about Z so the insert was facing upward and bored on the top of the bore. The problem is that Mastercam reversed the spindle direction and there was not way to fix it without creating a new incorrect tool definition of hand editing the posted code. In Mill there is a box where you can reverse the spindle from CW to CCW, the programmer has that control. I can run a right handed end mill backwards if I so desire, it is up to MEEEE! I can't thin of a reason I would want to do that but there might be a time where it will save my xxxx. In lathe it isn't even an option and it is extremely frustrating. Don't try to make the software too smart folks... You tie my hands behind my back.
c80f0f1006