Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.
Showing results for
Show only
|
Search instead for
Did you mean:
This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.Translate
I would like to see an option for even step downs in rough turning and boring. The current method of reducing the final 2 rough passes in not a good solution and prevents breaking a chip on 2 passes.
I would prefer to have the option to decided if it should equalize cut by dropping one pass and increasing all pass or add and pass and decrease all passes.
We need to dictate the EXACT step down depth, to control chip breakage. Having the program try and guess at what the best depth should be does NOT work, and with NO way around this option, it really really needs to go away ASAP please.
Many of us have spent massive amounts of time trying to figure out how to clear huge bird nests from parts, because of this terrible added feature. Most comical part of this is that roughing was almost perfect a year ago before this feature existed!
@Anonymous I would have to disagree just a little. I hope they put some logic into it. There are better ways than just explicitly following a stepdown value.
I think there should be the option you mention but needs to have some others and would be nice to have it fixed once and for all since it really is a core function and should have been working properly before adding more to turning. The problem is there is little public discussion these topics before there are released. I am not really sure why it was changed I assume it was a suggestion to keep from having a .001" doc on roughing pass. But there are better ways than this one.
That said, as it was before even if you did have a .001 pass, that .001 stringer was not enough to do damage. I was so used to altering step-downs in roughing to make the last pass +/- .002 or something, or the last pass .004 less depth, which would still generally break chips.
The logic in roughing I would think would be things like No-drag, Interrupted cuts, etc. No-drag is SUPER awesome. Roughing step downs though I'm just not sure why the step down value needs to be altered from what we dictate the program to do.
@Anonymous I understand what you are saying about wanting to have it follow a set step down. I cut materials that can be a real bear to break a chip on also. However there is typically a little wiggle room on the DOC. I personally think they should keep the way you are saying and follow a strict stepdown if that is what the user wants.
I believe however there are also some better methods that could be used that could automate the process a little and still provide good results.
In the example I will assume all radial dimensions for ease. Lets assume you have .4" to remove from od and you want to take 4 passes at .1 DOC each. That is pretty simple and you could do the math in your head pretty easily. Now lets assume you still have the .4 and you want to leave .03" for finish so you only need to remove .37" How would you handle this? 3 cuts at .1" and one at .07"? I would personally like 4 cuts at .0925, which is very close to the the .1" DOC I specified.
Now in the example lest say you have .45" to remove and you want to leave the same .03" for finish, now you have .42" remove with the roughing operation. So you could make 4 passes at .1" doc and one at .02". I would personally prefer 4 passes at .105" DOC
So these are pretty simple examples and the math is easily done in your head, but I don't want to have to do the math every time I decide I want to change how much stock I leave for finish or rough operation I do. In a real world example the number are typically not a clean to work with. I am running a right now that stock is 6.045" with the smallest diameter are 4.3315". I want to leave some for a finish tool also. I don't want to fiddle around with DOC calculations to create this operation. I also don't want a .001" cut at the end that is just basically wasting time and rubbing on my roughing tool.
The calculations are pretty simple and if they can create a kernel for adaptive clearing then a solution to rough turning stepdowns should be pretty easy for them.
So one solution I have used in other systems is to have on option to do exactly as you say. I enter a DOC and it follows it until it runs out of stock and the last cut is typically small. I can adjust the DOC and tweak it to get something I am happy with. I also have the option to select "Equalize by Increase DOC" or 'Equalize by Decrease DOC" . This results in basically the use even stepdowns setting in milling.
Another possible solution is to have the ability to specify the max and min DOC and have the algorithm attempt to adjust cuts to stay with in the parameters. This could be either hard numbers or percentage of DOC specified. The reality is if I break good chips at .1" DOC, I will also likely break chips from .090".110". As long as the tool path stays in the at DOC range I would be happy.
There are also other things to consider that I hope they take into account. I don't know the answers to these but hope they at some point have a discussion about them to input from users more qualified and with different experience then me.
One issue is that there typically tends to be a lighter pass at some point. Most CAM software I have used start with the first pass at full DOC and keep stepping down until the last pass ends up a lighter pass. Would it make sense to do the reverse and make the first cut the lighter and all subsequent passes at full DOC? This would allow for materiel variations without ending up with a heavy first cut.
Another issue is when there is an edge break chamfer on the end of the turned diameter. Since the lower diameter of the chamfer is taken into account in the roughing stepdown you typically end up with a lighter cut. If you are cutting the last pass at .1" and have a .03" chamfer the cut after the chamfer will only be .07" Could the chamfer be ignored then cleaned up at the end.
What about a shaft with multiple diameters, each diameter may could use a slightly different stepdown with in a specified range to achieve a good chip break.
Overlap passes in roughing needs looked at also. When machining thru a part I don't need to drag the insert over the stock as there is none there.
Another option is to rough out at full DOC leaving a stair step then on single "clean up cusp" type pass.
I am not saying these are all great or even good ideas, but they should be discussed before being implemented.
In the end most important, I agree we as the machinists should be able to help guide what the program designers are implementing.
It almost seems if there was a "Smart Roughing" check box or something, and when we decided to used it, it would calculate even steps to finish height, based on one single maximum roughing step down figure given. Seems that would be easy to implement and design.
One thing I would like to see is feed reduction when grooving is checked/used in roughing. Often when my VNMG insert plunges into the stock on the backside of a feature, the inserts sure do not like being driven in to 17-4 stainless at .013"IPR to a .1" depth. If there was a slower plunge rate before turning laterally inserts wold be kept much more happy.
