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
When creating a new tool in the tool library there needs to more parameters to allow for the use of high feed tools ie: Sandvik 419, So far I have used Form Tool but this only works for 2D operations, I have also tried Facemill and Tapered mill with no success.
Yes most tooling companies do provide an effective or programmible radius but to be honist using a chamfer mill better defines these parameters , Tools such as the Sandvik 419 or Taegutec TF90 are essencially chamfer mills with corner radius's. I have achieved the tool form I require with chamfer and facemill only problem is I get an Error: Tool cannot reach tapered wall. or Warning: Empty toolpath.
We conduct 60% of our work with highfeed mills ranging from 12-100mm, So it would be nice if the autodesk team could tidy this up.
I have also always used the bull mill for a feed mill definition, but I use them rarely and could see where a low-angle chamfer mill with corner radii could be more useful, especially for rest machining operations.
I really think we need to be able to use a form tool for every operation properly.
There are a lot of people that use the high feed mills for roughing and semi-finishing. Which means you also need to be able to use these in 3D Finishing Operations.
I have some high feed cutters laying around that don't get used because the system doesn't support them. You can make them cut chips with defining them as bullnose, or chamfer mill for example but that means the simulation is wrong, rest stock calculation is wrong, feeds&speeds calculations are wrong, assumptions on what the tool can do are wrong etc.
So no that is in no way sufficient to use these tools properly.
HI CJ, I also have found that the defining a high feed tool as a bullnose does not work well. I have to define the tool I am using as a bullnose with a .300 rad. to get the bottom to clean up. But if I have to machine around a boss or shoulder the first few depth passes will gouge the part because the code is being calculated from the .300 rad and the tool is not a true .300 rad. I have to remember to leave an extra .060 stock on the side and then come back in with a different tool to finish cleaning up the wall.
I use both Fusion and Inventor HSM on a daily basis and I believe this is a need for the product and not a want, In the interim either allow chamfer mills to preform all machining operations and or form mills.
Without sounding sarcastic I do use Inventor HSM (High Speed Machining) There for we need to define High Speed/Feed Tools.
I am currently programming a part using a 52mm Sandvik 419 the difference between the actual insert profile and the programmed radius 5mm is .61mm there for I have to force the tool to gouge to produce the correct form. I like living life on the edge but not with a million dollar machine.
I agree with @Laurens-3DTechDraw. All operations should be able to use a mill that you like to use.
Also multiple feeds & speeds for a tool is a big wish.
Maybe something to trigger by selecting a material to the component so all feeds & speeds are set directly correct for all operations in that specific part.
We use HSMWorks daily for mill and turning, the parameters for tool definition are definitely limited, modelling a tool exactly as it is without work-arounds would be great.
If we could define a tool as a bullnose and also give it a tip diameter I think it would take care of the issues I am having. The tool I am using would be defined as a 2.000 bullnose with a .090R and a tip dia. of 1.400. Then the system could use the .090R for the 3-D and adaptive calculations and the 1.400 tip dia. for bottom clean up.
@Anonymous Is the tool you are using a true high feed cutter, If it is then most are normally defined by a minor diameter an angle a major diameter and corner radius, Then reason for this post is I have just finished a job using a sandvik 419 and I had to force the tool to gouge by .61mm in order to generate the correct profile on the part.See photo below to why we need to control over the tool profile.
Hi precisionworkz, yes we are using true high feed inserts. So far mostly for adaptive facing. In that case I have had to use a larger radius than the manufactures program radius to get the face to clean up. I am going to try defining the tool two different ways, one with the larger radius for facing and another with the manufactures program radius for 3-D. We will se how that goes.
Hi @jasonsXXW8Q you can define the correct profile using chamfermill or facemill this will work for your adaptive facing operations you will then have to define a 2nd tool (as mentioned) in you library as a Bullmill to conduct your 3D operations.hmmmmm
