5 Axis Toolpath Problems

[xform precision creations]

I am having a great difficulty getting the desired result from my 5 axis tool paths. My machine is a Thermwood 67. I have machined a test part to learn on, using 3D pocket tool paths and have programed some 5 axis toolpaths which should run over the 3D surface and just touch the already machined surface. I am doing this as verification just to check I have all the 5axis parameters correct. The result I get is miles different from what it should be. Trouble is that when I backplot and verify everything looks fine but the actual result is up to half a cutter diameter, different but not in any pattern to suggest that I am compensating to the wrong side etc. Any help would be most appreachiated since I have spent all day playing around with different settings(mainly the comp settings and tip and centre settings as I thought that it was most likely to be these) but get all sorts of diffenrent results none of which are correct. (but they all look correct in the backplot, which is a bit of a worry). I am not sure what to do next. This newsgroup is my only help since I have found that even though we have paid Mastercam maintenance, it doesn't actually entitle you to any help.

Thank you.

[cadcam]

Xform, do you have the sample file you are playing with?

This would be helpful.

 

Now you are saying that looks correct on the back blot correct ?But the output to the machine is other wise.

 

I am leaning from just what I have at this time towards your post.

were did the post come from?

 

Are you trying to use one of the 5 axis options and get the tip control from a floor surface that has all ready been cut?

 

Just a few thinks to move this along.

[gcode]

Howard,

Are you using a proven post?

Check out you Tip Control settings in 5XCurv.

"On Projected Curve" and "Comp to Surfaces" can give entirely different results.

Under most conditions, I use the 3d curves to define a toolpath, "Tool Axis Control" to the surface and "Tip Control" to the surface.

If you are using the "Entry/Exit" options, review them carefully. They can have unexpected results if you are not used to them.

The resident Thermwood experts havn't checked in yet this morning, but they'll get here.

 

[ 04-10-2004, 11:29 AM: Message edited by: gcode ]

[Charles Davis]

It can one of a few things:

1. You post is not correct.

2. You are not using the post correctly. Remember, changes in tool length affect the code on some 5-axis machines. If the post does not know the tool length, it can' calculate correct code.

 

If you don't understand what I just said, then you are woefully unprepared to start programming this machine.

[Jimmy Wakeford from Barefoot CNC]

+1 Charles.

 

If the angles look correct then I would suspect tool length issues. The post being used is either asking for tool length while posting or getting it from the overall tool length parameter for each tool.

[xform precision creations]

Sorry I havn't replyed to your questions earlier but have been away for a day. The Thermwood post I am using is from CNC Automation.

I have verified the ref tool length with a simple program where I machined a simple contour path from above, then rotated the B axis 90degree so that it came in and machined the same surface that was cut with the contour path and it was perfect. Also accuratly measured the length from pivot of B axis with machine cooridnates and DTI gage. I am therefore 100% sure the tool length is correct.

I have worked out what is actually happening now. The part is a simple top third of a sphere with a flat plane at the bottom. It is a flow5axis path radiating from the top centre and tool is remaining normal to surface at all positions (no axis limits set or anything like that). Tip is selected for Tip comp. The path it generates is therefore touching the surface as it goes radially from the centre stopping by 1/4" above the flat comp surface plane at the bottom (as it should because it is a 1/2" ball nose cutter). SO everything looks fine here. What it accutally cuts is it is touching at the top as it should but as the tool moves down the tool path, it starts digging into the part and stopping 1/4" above the bottom plane. At this bottom point the lowest tip of the ball nose tool is on the tool path and therefore has cut into the part by the tool radius. Therefore also stopping 1/4" above the plane since this is the tool path stop point. So the bottom tip of the tool is following the toolpath and ignoring the radius of the cutter as though it was referencing to the top tool plane even though the tool motion remains normal to the surface. I am thinking that it could be something to do with the T/C plane settings for the path and will try changing them.

I hope this decribes the problem clearly. If not I could put the file on the site for someone to have a look at. You might have to tell me how to do this. Thank you.

[Jimmy Wakeford from Barefoot CNC]

Use comp to surfs and select your cut pattern

[xform precision creations]

Have alreeady selected the appropriate comp surfaces the comp to surfaces. Problem is that it looks exactly right when backplotting and verifying. It is only when you machine the part that problems show up.

[crazy^millman]

Put the file on the FTP. I would also be checking to make sure that in your misc for that post that you have retract to limits and to null and other things that the post uses for it clearence point are being done correctly and set correctly for that post. I would also look at the settings of the arc moves by the post also. I do not like the fully locking of the post they offer and well you are pretty much at the mercy of the post and who supports the post to get anything tweaked. PC will kick in now and I will shut my mouth about what I think about that.

 

I do all kind of crazy things here and think this is just a post issue. I am using the MP5AXGEN now and still have things to get tweaked as far as clearence issues go but as far as making the paths I want to problems what so ever. Be nice to unlokc the psb to make thing go the way I want but then what fun making my life easier be.

[Keithm]

Is the machine in tram? I ran a thermwood and the A or B axis would come out of tram very easy. that could cause you some problems

[MATT Q]

Have you got a hold of CNC automation on this issue? sounds like a post issue or the head is not zero'd in

[Code_Breaker]

Millman,

 

Is MP5AXGEN a "provided generic post"? If so, where can I get a copy?

 

 

Code_Breaker

[cadcam]

code _breaker it's on you mastercam disc or if they installed all the post in the install it's in the post libary.

[crazy^millman]

Jay provides the answer.

 

Thing about this post is very genric and I have heavy modifications to the one I am still getting to work good on the machine here. I had soemthing close but went this route ni hopes of gettign exactly what I want but may get the old start from scratch one going soon. Have got some good clues where to start but the vectors and the cabs are going to give me some trouble since I am not previalge to the certain information I need and will have to pull alot of it out of the air so to speak. Good luck in your application think I got it easier than most no crazy G112 or axis mapping so might not be as bad as I think it will be.

[crazy^millman]

xform I put a simple examples of what I am saying on the FTP. One is called 5 AXIS SWARF EXAMPLE the other is 5 AXIS SWARF EXAMPLE2. I created an upper and lower circle and then create 16 points on each. I then create 2 other shapes keeping the points the same on the top and bottom. I then used the method I described above to get the perfect toolpath. I hope that helps.

[Code_Breaker]

I have these posts--MPGEN5X_FANUC.PST and MPGEN5X_MILLPLUS.PST. I was thinking maybe MP5AXGEN was another example.

 

Thanks

 

Code_Breaker

[xform precision creations]

Thanks everyone. Millman I will have a look at the files, thanks. I will try a couple more settings thismorning just to make sure I havn't forgotten something and if I still have problems I will put the file on the FTP site. While it sounds like it may be a post problem, I am wondering if it has something to so with the compenstaion direction setting, (left or right). I do not fully understand the meaning of this setting when it comes to 5 axis surface machining. I know that when 2D contouring etc it changes the side of the line you are on but maybe someone could describe its function in surface machining. I would have thought that the computer would have looked at the complete radius of the tool and compensated to that regardless of whether it is apporaching from the left or right?

[crazy^millman]

Sorry Code breaker me and my bad typing and spelling skills again.

[xform precision creations]

I have tried all sorts of settings and still arn't getting anywhere. I have posted the file on the FTP site. File is called SPHERE TEST.MC9 It is zipped up. Basically the 3D parrallel toolpaths machine the shape. The 5 axis path was just to verity if it is working correctly. You will notice that it backplots fine, it is not until you cut the part that problems show up in the 5 axis path. If someone could open the 5ax tool path parameters and see if I have set things correctly it would be most appreachiated. Thank you.

[crazy^millman]

Xform from what I can see you need to make the check surface not go completly under the sphere. I created a edge from the sphere and cut the surface out shoudl not matter but I have always had better result havign sufrace that are the shape to what I want verses a full shape for a check surface that goes into or through a part just seems to give Mastercam a fit sometimes. I might alos look at soild for a part of this nature I find alot of the toolpath works better when working with soild espically is doing oppsite side or cavities of parts. I looked at your 3rd op no check surface thtere so that will gouge. I also if doing 3d flat parts use depth as a boundary as well as check surface to keep tool from hitting surfaces. The op 4 look fince and does fine from what I can see and if that toolpaths is gouging on the machine I say it is a post issue and send this file to them and ask them to fix the problem if the machine is trammed in which I believe you said it was.

[xform precision creations]

Millman, Thanks for taking a look at the file. If I still have no luck I will send the file to the post peolple to take a look at.

What do you mean by the machine being trammed in? How do I check this? Can't find anything in the Thermwood books that talk about tramming.

[crazy^millman]

Well old school method of checkign the head on a Bridgeport was to check the head for tram to the table. The aligment method they are talking about in the book is what I am refering to. I put a 1/2 cardibe blank in the spindle. I then turn the 4th axis 360 degrees if I get more than .002 I realign the 4th and 5th axis till within my tolerance of no more than .002 but they allow .005 I have found that graet of a variance can cause probelms on certain toolpaths and try for within .001 on most of the setting producers for the machine. Yeah it is a real pian in the arse but to me is needed to make good parts. If the machine is out of tram or you do not have the correct povit distace for the post then problem can arise when doing 5 axis toolpath and can cause some very undesirable results. Hope that helps and is clear enough also put note in oyur book and I keep a log of all me measurement everytime I adjust the machine to see patterns. I knock on wood have not crashed this machine yet so only having a need for one .003 shim to keep in within my specifactions for the machine not Thermwoods .005 tolerence.

[xform precision creations]

I did a quick check on the allignment of the 4th axis by rotating 360degrees. Measured about 3/16" error! Looks as though this is the source of the problems. I will do a full head alignment as decribed in the book, trying to acheive the tolerences you suggest. Thanks.

[MATT Q]

That is the problem right there is that machine have a tool changer or is it a dual end spindle?

[crazy^millman]

WOW Yeah that is not good. Tram that bad boy but now I am worried I thought this was a new machine and is it was has it been crashed? When doign the 4th axis aligment be very very careful of the tension you put on those blot that material is very brittle and when our breakes and I know it will I am making a new plate out of 6061-T6 and getting away from that cast stuff they use. Good luck and keep us posted