problems with dxf

[thereclinerman]

here is the situation. retiring from the military and going to get a cnc machine to cut parts for furniture frames. trying out different software. plan on cutting out parts on 4 x 8 3/4 plywood. number of parts would be on sheet and then nested. toolpath generated and parts cut. do not have a cnc machine yet.

i downloaded a trial version of aspire 3. was able to design a part, nest it giving it the number of copies and create a toopath. the problem is, whenever i import a dxf a friend made in autocad, when i try to nest the part, it tells me no suitable vectors found. no vectors show as open and it will not make the number of parts needed. if i creat a part in aspire and import the dxf onto the same sheet, aspire will create muliple parts of the part created in aspire and them tell me it cant nest the part i imported.

in your opinion, is this software suitable for what i am trying to do? perhaps create the parts in autocad and use aspire 3 for toolpaths?

i have uploaded the dxf. any help in explaining how to do this is or pointing me in the right direction is greatly appreciated. thanks jim

[Robert Alexander]

here is the situation. retiring from the military and going to get a cnc machine to cut parts for furniture frames. trying out different software. plan on cutting out parts on 4 x 8 3/4 plywood. number of parts would be on sheet and then nested. toolpath generated and parts cut. do not have a cnc machine yet.

i downloaded a trial version of aspire 3. was able to design a part, nest it giving it the number of copies and create a toopath. the problem is, whenever i import a dxf a friend made in autocad, when i try to nest the part, it tells me no suitable vectors found. no vectors show as open and it will not make the number of parts needed. if i creat a part in aspire and import the dxf onto the same sheet, aspire will create muliple parts of the part created in aspire and them tell me it cant nest the part i imported.

in your opinion, is this software suitable for what i am trying to do? perhaps create the parts in autocad and use aspire 3 for toolpaths?

i have uploaded the dxf. any help in explaining how to do this is or pointing me in the right direction is greatly appreciated. thanks jim

I could not import your DXF file into my CAD program or Aspire. In your friend's Autocad check to see if the lines are set to hairline and there are no extra layers. You only need 1 layer turned on for 2-D drawings. A lot of times other Autocad files have multiple layers,which can cause problems when you import them into other programs.

As for using Autocad for making your drawings it's a monster[book] of a program. If you have Autocad already on your computer, and you are comfortable using it stay with it. Other wise get a simple 2-D cad program for doing your design work. I use AutoSketch for all my design work, and then I import my drawings into Aspire. Hope this helps

[copperhead4321]

http://best in aspire I was able to open your dxf file in aspire 3 just having trouble sending a pic to you

[Mick Martin]

I was able to open the DXF into Aspire

You could create this direct in Aspire - Below is how to import a DXF into Aspire

- Start Aspire.
- Click on the Icon "create a new file" - I used 16" wide by 20" high since you part fitted into this size.
- On the drawing tab click on "import vectors from file'.
- select all you lines - click and hold the left mouse button off your project then drag a square to the lower right hand corner. This will select all your lines.
- Click on the letter "J" on your keyboard to join all the open lines, in the join dialog box enter .010 then click join.
- Select or your line again, this time click on any line, since will select your project since they are all joined together.
- Click on the Icon "switch to toolpath tab" on the drawing tab - third row last Icon on the right. - a new window should open on the right hand side of your screen.
- With your lines selected click on the Icon "create profile toolpath"
- It might ask you to check your material if it does click on OK
- Start depth = 0, cut depth plus Thickness of your material plus .020" to ensure your bit cuts through the material.
- Choose your router bit, I used .25" straight end mill.
- In the machine vectors section click on "outside / Right"
- Click on Calculate
- Click on "preview toolpath"
- to save this file click on "File" upper left hand corner of the screen, then save as ............

I hope this helps

Note - Since this is a trial version you will not be able to create a toolpath to send to the CNC .......... I think, not to sure about this.

Mick

[fixtureman]

I can open it in both aspire and autocad I did notice that the bottom leg is larger than the top leg
Bottom = 5.6681 tall
top = 5.4765 tall

the top cutout is 5.9197
the bottom cutout is 5.7786

something doesn't seem right

[thereclinerman]

thanks for all the help. this part is just a made up sample to try different things on. mick, i followed your examples and what you said worked perfectly. thanks. i open the background as a 48 x 96 as this is the size of the wood. in order to make mutliple parts of this and nest it, i selected the part, clicked on nest and when the next tab opened, i filled it out and set the number of parts to 20 and then clicked on nest. this it when it said no suitable vectors found. do i need to manually creat 20 parts by copy and paste or am i not understanding something. thank to all

[Joey Jarrard]

Did you have the object selected. If so the lines making the part that came from autocad may be broken or have difrent z nodes. If there are depth to the file brought over v carve or aspire will not see it as a complete vector. I use autocad every day with aspire and it works great. When I am in front of my pc with autocad I will take a look at it.

[Mick Martin]

Did you have the object selected. If so the lines making the part that came from autocad may be broken or have difrent z nodes. If there are depth to the file brought over v carve or aspire will not see it as a complete vector. I use autocad every day with aspire and it works great. When I am in front of my pc with autocad I will take a look at it.

The lines were not joined, they were all single lines, that's why I wrote above in my comments to join them.

Mick

[thereclinerman]

mick, i am going to get another dxf sample made to play with. will make sure vectors are closed. thanks

joey, can you make a t-bone or dog-bone with autocad. the guy who made my sample is in california and its hard to communicate. he was just teaching/showing me how to do some stuff. guess i will have to try to learn autocad or auosketch. thanks

[Joey Jarrard]

Acad will do it but you will have to draw it using fillets. Aspire has a beter set up for doing this.

Take a look at the pic. It is a great setting that makes it real easy to do dogbone and Tbone's for slots.

[Robert Alexander]

I was able to open the DXF into Aspire
Mick

Mick did you do a direct import into Aspire 3? I could not figure out how you were able to get it open at first. After opening the zip file I moved it into a different file folder, then I was able to open it in Aspire3 with no problems. My computer is weird sometimes, or maybe it's just the operator.

[fixtureman]

I opened it right from the web site in Aspire

[stinger23]

this dxf was created with mastercam x4..

it is written in the file.

[Mick Martin]

After opening the zip file I moved it into a different file folder, then I was able to open it in Aspire3 with no problems. My computer is weird sometimes, or maybe it's just the operator.

Hi Robert,

I opened the Zip file and moved it into a new folder, then into Aspire just the way you did.

Mick

[Dennis]

I use autocad regularly. In 2010 I select Edit Polyline, input M (for multiple) and hit enter, select all the parts and hit enter, select join and hit enter, if fuzz comes up as a choice, hit enter. When you select any portion of the object it will be a solid line which is a closed vector. When you open it in Aspire it should be ready to cut. I prefer to do the "dog boneing" in Aspire as well.

I always check for duplicate vectors and open vectors usinf the edit menu.

If, per happen chance, you get an open vector in Aspire, you can click on the node edit button, look for the green node (assuming there is one open space) and check to see if it is not connected. I check by dragging it aside and then doing undo. There are several was to weld it closed. An easy way is to drag the nodes across one another and use the scissors but there ar others in the program.

[Joey Jarrard]

Dennis that was a great post. It is the same steps I do for all my parts. Keep it up. [fantastic]