Announcement

Collapse
No announcement yet.

Center Cutting & Non Center Cutting Tools in Turbo HSR.

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Center Cutting & Non Center Cutting Tools in Turbo HSR.

    Of late we have been receiving questions about TurboHSR ability to handle Non-Center Cutting tools. This is the place where we can define if the tool we are using has the ability to do center cutting or not. Look at the image below :

    https://solidcamail-my.sharepoint.co...fzsFQ?e=IOziNX

    There have been a lot of misconceptions about what constitutes center cutting & what does not. For us to understand that, we need to understand the tool geometries. Look at the following Figure.

    https://solidcamail-my.sharepoint.co...RY1tg?e=GSWbm7

    Solid Carbide Endmills can be center cutting and non-center cutting. As their name implies, center cutting end mills have cutting edges on both the end face of the cutter and the sides. Center cutting end mills are essential for plunge milling.

    Non-center cutting end mills have cutting edges only on the sides and are used only for side milling. These tools are identified by a small hole at the center. These tools cannot be used to ramp or directly plunge into the material. These tools can either approach the stock from outside or need a pre-drilled hole to enter the stock.


    https://solidcamail-my.sharepoint.co...HDtdg?e=byCVtW

    For inserted carbide tools, it is a different story. Most of the tools (Especially the round insert tools) can plunge or ramp only to a certain depth with a certain angle (As defined by the manufacturer). From a theoretical point of view, these tools come under the classification of non-center cutting tools as they do not have any cutting edges in the center. However, they can ramp or plunge as per the cutting manufacturer's parameters.

    Coming back to Turbo HSR, we handle both these situations in a different way.

    Situation 1 – User has defined a non-center cutting Solid Carbide end mill :

    In this situation, it is clear that this tool cannot plunge or ramp on the material. It can enter the stock from outside by taking the depth of cut in air or the user must provide with a pre-drilled hole and the tool will enter the stock in the predrilled hole. In this situation, the user must do the following.

    Disable center cutting option in THSR.


    https://solidcamail-my.sharepoint.co...Zn1ig?e=diZ611

    Next is to disable the “use ramp” options in linking (This will be automated in future releases).

    By doing this, SolidCAM THSR will calculate only those areas/regions where the tool can approach the part from outside the stock. It will leave out areas/regions where it would be necessary to either ramp or plunge into the stock (unless a pre-drill is already defined).

    Situation 2– User has defined a non-center cutting Solid Carbide inserted end mill :

    Like we explained before, these tools although fall under the non-center cutting tools, can ramp or plunge only to a certain depth. This depth is defined in the “Depth of Cut” section of the toolpath. The user needs to enable the “Center Cutting Tool” as shown below.


    https://solidcamail-my.sharepoint.co...5LV_g?e=RGJQM6

    The user also needs to enable “Use Ramp” in the links section (again like we said this will be automated in future releases).

    However such tools (Inserted carbide end mills) have a limitation that they cannot ramp in extremely tight areas (Like small holes, pockets, etc which are slightly bigger than the tool diameter). This is because when the tool enters such tight areas where it cannot move much in the Radial direction (XY Plane) the center material is getting formed. Observe the figure below.


    https://solidcamail-my.sharepoint.co...axL2g?e=vIGtMU

    You can see the center material is getting formed and is entering the relief in the cutting tool. If the tool does not get enough movement in the XY plane this material could keep building and eventually collide with the soft part of the tool & damage it. To prevent this the user needs to specify the max diameter/diagonal length that SolidCAM should look for in order to prevent the above situation from arising. This can be found under Passes ==> Smoothing ==> Filtering.

    https://solidcamail-my.sharepoint.co...Ra0-g?e=1IEGzH

    We hope that this post clarifies the center-cutting and non-center-cutting questions that have been asked to us over time. If there are questions please let us know so that we could answer the same.

    Amod Onkar
    3x and sim5x product manager
Working...
X